It
•£ 1 No. FHWA/RD80/027
H H WA 
8002 /
W STRUCTURAL SYSTEMS FOR
ZERO MAINTENANCE PAVEMENTS
Vol. 2. Analysis of Anchored
Pavements Using ANSYS
August 1980
Final Report
DEPARTMENT OF
RANSPORTATION
JAN 1.4 Mil
LIBRARY
"%■* *
Document is available to the public through
the National Technical Information Service,
Springfield, Virginia 22161
Prepared for
FEDERAL HIGHWAY ADMINISTRATION
Offices of Research & Development
Structures and Applied Mechanics Division
Washington, D.C. 20590
FOREWORD
This report provides a set of procedures to evaluate the response of an anchored
pavement subjected to static vehicle loads, moisture variation in the subgrade,
and/or temperature variation through the surface of the pavement. Basically,
these procedures consist of the use of two computer programs known as FEMESH and
ANSYS. The FEMESH program divides the analytical model into a set of rectangular
elements and the ANSYS program evaluates the stresses, strains, and deflections
at each of these elements in each material included in the analytical model.
The procedures are versatile and capable of solving geometrically complex
structures on a geologically complex earth mass.
This report is the second volume of a set of three final reports resulting from
a research contract, "New Structural Systems for ZeroMaintenance Pavements,"
issued to Dames & Moore by the Office of Research and Development of the
Federal Highway Administration. The objective of this research study was to
identify and assess the potential of new and innovative structural concepts
and systems to serve as "ZeroMaintenance" pavements. An interim report,
"Unique Concepts and Systems for Zero Maintenance Pavements," FHWARD7776,
provides an updated stateoftheart and comprehensive review of each of the
three major structural components of a pavement system: the subgrade, the base
and subbase, and the pavement surface. The other two volumes in this final set
are reports FHWA/RD80/026, Volume 1: Analytical and Experimental Studies of an
Anchored Pavement, and FHWA/RD80/028, Volume 3: Anchored Pavement System
Designed for Edens Expressway. Volume 1 was published and distributed
previously.
Copies of Volumes 2 and 3 are being distributed jointly by a single transmittal
memorandum primarily to research and development audiences*^
Charles F. Scheffey 1/
Director, Office of Research
Federal Highway Administration
NOTICE
This document is disseminated under the sponsorship of the Department of
Transportation in the interest of information exchange. The United States
Government assumes no liability for its contents or use thereof.
The contents of this report reflect the views of the Dames & Moore organization
which is responsible for the facts and the accuracy of the data presented
herein. The contents do not necessarily reflect the official views or policy of
the Department of Transportation.
This report does not constitute a standard, specification, or regulation.
The United States Government does not endorse products or manufacturers.
Trademarks or manufacturers' names appear herein only because they are
considered essential to the object of this document.
y
.A3
Technical Report Documentation Page
1. Report No.
FHWA/RD80/027
2. Government Accession No.
3. Recipient's Catalog No.
4. Title and Subtitle
NEW STRUCTURAL SYSTEMS FOR ZEROMAINTENANCE PAVEMENTS
Volume 2: Analysis of Anchored Pavements Using ANSYS
5. Report Date
August 19£0
6. Performing Organization Code
7. Author's)
8. Performing Organization Report No.
S.K. Saxena and S.G. Militsopoulos
9. Performing Organization Name and Address
Dames & Moore
7101 Wisconsin Avenue
Washington, D.C. 20014
and
Illinois Institute of
Technology
Civil Engineering Department
Chicago, Illinois 60616
10. Work Unit No. (TRAIS)
FCP 35E2042
11. Contract or Grant No.
DOTFH119114
12. Sponsoring Agency Name and Address
Offices of Research and Development
Federal Highway Administration
U.S. Department of Transportation
Washington, D.C. 20590
13. Type of Report and Period Covered
Final Report
14. Sponsoring Agency Code
15. Supplementary Notes
FHWA Contract Manager: Dr. Floyd J. Stanek (HRS14)
Dames & Moore Project Manager: Dr. Mysore S. Nataraja
DEPARTMENT OF
TOANSPORTATfON
i6. Abstract New Structural Systems for ZeroMaintenance Pavements. The purpos* of this
study is to investigate the feasibility of designing and qons^nlctJiRg'^gsiteFfective
"ZeroMaintenance" highways.
Volume 2: Analysis of Anchored Pavements Using ANSY
which provides a set of procedures to evaluate the respon
subjected to vehicle static loads, moisture variation in the subgTa^eT^rntr7^r temper
ature variation through the surface of the pavement. These procedures include two
computer programs known as FEMESH and ANSYS. The FEMESH program generates rectangu
lar meshes in either a two or three dimensional coordinate system for any prespecifiec
number and spacing of nodes. The ANSYS program evaluates the stresses, strains, and
the deflections at all elements in each material included in the analytical model.
The program can be used for any number of different materials in any direction. In
the analysis of heat transfer, the program provides the distribution of temperature
as a function of time at predesignated points. The program is versatile and capable
of solving complex geometrical structures supported on a geologically complex earth
mass. The behavior of an anchored pavement section is evaluated with sets of
computer programmed mechanistic models. The manual was written to minimize reference
to other publications.
This volume is the second in a series. The others in the series are: Volume 1:
Analytical and Experimental Studies of an Anchored Pavement, and Volume 3: Anchored
Pavement System Designed for Edens Expressway. Abstracts of these volumes are
included on page ii of this volume.
. ThissfT^iDprt is ja manual
Ulan anchored aavement
17. Key Words
Anchored pavement
pavement systems
FEMESH and ANSYS
18. Distribution Statement
No restrictions. This document is avail
able to the public through the National
Technical Information Service, Springfield,
Virginia 22161.
19. Security Classif. (of this report)
Unclassified
20. Security Classif. (of this page)
Unclassified
21. No. of Pages
144
22. Price
Form DOT F 1700.7 (872)
Reproduction of completed page authorized
Abstracts of Related Documents
Volume 1: Analytical and Experimental Studies of an Anchored Pavement :
A Candidate ZeroMaintenance Pavement
This report documents an investigation of the design feasibility and
construction costeffectiveness of an anchored pavement concept for zero
maintenance highways. An analytical model is designed to verify computer
program results and to investigate construction methods for a fullscale
highway section. The purpose of the analytical study is (1) to present
thermal, mechanical, and thermomechanical properties of typical materials
in a form easily adaptable to computer programs, and (2) to describe
environmental and mechanical properties of a conventional slab and an
anchored pavement in both continuous and jointed configurations. The two
pavements were subject to heat transfer, thermal stress, and mechanical
stress analyses. The anchored pavement offers two distinct advantages
over a conventional pavement—deflections are lower and more uniform, and
stresses in the soil are lower and distributed more widely by the rigid
anchors. Subgraderelated failure is less likely to occur if loads are
transmitted deeper within the subgrade. Threedimensional finite element
analysis is considered to be the most efficient technique for examining the
significance of environmentally induced stress. The use of the finite
element method is anticipated as more advanced analytic techniques are
developed.
Volume 3: Anchored Pavement System Designed for Edens Expressway
This report provides an analysis example of an actual pavement and the
cost estimate using the anchored system. The actual pavement is the Edens
Expressway in Chicago. The report provides the response of the Edens
Expressway subjected to mechanical and environmental loads using the an
chored pavement concept. The mechanical and thermal properties of materi
als that could be encountered in future reconstruction of Edens Expressway
are presented in a consistent form for computer programming. These proper
ties are viewed as typical design values during investigation of pavement
response. The behavior of the anchored pavement under induced temperature
loads and weakening of subgrade (by thawing action) is clearly demon
strated. This report will enable application of the anchored pavement
concept by any road with heavy traffic. The example problem provides the
input parameters of materials and loads for the analysis, the generation of
finite element mesh, and the results of the analysis. The computer program
ANSYS was used for this study (the manual for the use of the program is
presented in Vol. 2 of this series of reports).
TABLE OF CONTENTS
CHAPTER 1 INTRODUCTION 1
1 . 1 OBJECTIVE . 1
1 .2 SCOPE 1
l'.2 RELATED 'DOCUMENTS* .................... i
CHAPTER 2 ANALYSIS PROCEDURE 3
2.1 COMPUTER CODES USED 3
2.2 PREPARATION OF COMPUTER INPUT 3
2.2.1 System Control Cards 3
2.2.2 ANSYS Problem '. . 5
2.2.3 LoginLogout Procedures for 3atch Users 5
2.2.4 Remote Batch Terminal Commands 7
2.3 ANALYSIS METHODS ; 3
2.3.1 Static Analysis 3
2.3.2 Heat Transfer 10
2.4 LOAD CHARACTERISTICS 1Q
2.5 MATERIAL CHARACTERIZATION 11
CHAPTER 3 OPERATING INSTRUCTIONS FOR FEMESH . . . 22
3.1 FEMESH SOURCE CODE 22
3.2 INPUT DATA 22
3.3 MESH GENERATION EXAMPLE 30
CHAPTER 4 OPERATING INSTRUCTIONS FOR ANSYS 36
4.1 WAVE FRONT SOLUTION AND LIMITATIONS 36
4.2 DATA INPUT INSTRUCTIONS 37
4.2.1 ANSYS Input Data for Static Analysis 38
4.2.2 ANSYS Input Data for Heat Transfer Analysis .... 51
4.2.3 ANSYS Input Oata for Thermal Stress Analysis ... 57
CHAPTER 5 ELEMENT LI3RARY OF ANSYS '. 60
5.1 ELEMENT SELECTION 60
5.2 ELEMENT LIBRARY FOR STATIC ANALYSIS 60
5.2.1 Threedimensional Isoparametric Solid Element ... 60
5.2.2 Threedimensional Interface Element 62
m
Page
5.3 ELEMENT LIBRARY FOR HEAT TRANSFER 64
5.3.1 Isoparametric Quadri lateral Temperature Element. . 64
5.3.2 Twodimensional Conducting Bar 6°
5.4 ELEMENT LIBRARY FOR THERMAL STRESS ANALYSIS 67
5.4.1 Twodimensional Isoparametric Element
57
5.4.2 Twodimensional Interface Element 68
CHAPTER 5 CONCLUSION 94
REFERENCES 95
APPENDICES 97
A. NOTATION 97
8. ANALYSIS PROCEDURES 98
C. ELEMENT LIBRARY 107
D. COMPUTER DEFINITIONS AND COMMUNICATION LINKS .... 130
TV
LIST OF TABLES
TABLE Page
2.1 EQUILIBRIUM EQUATIONS CStatic Analysis) FOR
AN ELEMENT .,.,.,,..,, 12
2.2 EQUILIBRIUM EQUATIONS (.Thermal Analysis) FOR
AN ELEMENT . . . , . , . 13
2.3 .MATERIAL PROPERTY NAMES 14
2.4 .MATERIAL PROPERTIES VERSUS ELEMENT SUBROUTINE 15
4.1 ELEMENT REORDERING INSTRUCTIONS ..... 57
4.2 ELEMENT REORDERING FOR SAMPLE PROBLEM 58
5.1 ELEMENT SUMMARY TABLE 71
5.2 INPUT OF ELEMENT PARAiMETERS ON ANSYS PROGRAM DATA CARDS. 73
5.3 UNITS OF INPUT AND OUTPUT PARAMETERS 74
5.4 ISOPARAMETRIC SOLID ELEMENT  THREEDIMENSIONAL 75
5.5 ISOPARAMETRIC SOLID ELEMENT  THREEDIMENSIONAL ELEMENT
PRINTOUT EXPLANATIONS 77
5.6 INTERFACE ELEMENT  THREEDIMENSIONAL 79
5.7 INTERFACE ELEMENT  THREEDIMENSIONAL ELEMENT PRINTOUT
EXPLANATIONS 80
5.8 ISOPARAMETRIC QUADRILATERAL TEMPERATURE ELEMENT 81
5.9 ISOPARAMETRIC QUADRILATERAL TEMPERATURE ELEMENT 
ELEMENT PRINTOUT EXPLANATIONS 81
5.10 CONDUCTING BAR  TWODIMENSIONAL 82
5.11 TWODIMENSIONAL ISOPARAMETRIC ELEMENT 83
5.12 TOODIMENSIONAL ISOPARAMETRIC ELEMENT, ELEMENT PRINTOUT
EXPLANATIONS . . . . . 85
5.13 INTERFACE ELEMENT  TOODIMENSIONAL 86
5.14 INTERFACE ELEMENT  TOO DIMENSIONAL ELEMENT PRINTOUT
EXPLANATIONS 87
LIST OF FIGURES
FIGURE Page
1 .Soil Structure Interface Connection 2
2.1 Arbitrary Rectangular Mesh Generation 16
2.2 ANSYS Setup Deck, for CDC Computer 17
2.3 Cufaer 176 Configuration . . . 13
2.4 Summary of ANSYS Analysis Types 19
2.5 Static Load Model (Dimensions and Load Will Vary With
Vehicle) 20
2.5 Temperature Load Model 21
3.1 Example of Mesh Generation 31
4.1 ELxample of Element Reordering to Minimize the Wave
Front 59
5.1 ThreeDimensional Isoparametric Solid Element .... 88
5.2 ThreeDimensional Isoparametric Solid Element Output. 88
5.3 ThreeDimensional Intarfaca Element 39
5.4 Three Dimensional Intarfaca Element Output 89
5.5 Isoparametric Quadrilateral Temperature Element ... 90
5.6 TwoDimensional Conducting Bar Element 91
5.7 TwoDimensional Isoparametric Element . . 92
5.8 TwoDimensional Isoparametric Element Output 92
5.9 TwoDimensional Interface Element 53
5.10 TwoDimensional Interface Element Output 93
VI
CHAPTER 1
INTRODUCTION
i . 1 OBJECTIVE
The objective of this manual Is to provide the pavement analyst
with a ready reference of procedures to obtain the response of an
anchored pavement subject to vehicle static loads, moisture variation
of the subgrade, and temperature variation at the surface of the pave
ment.
1.2 SCOPE
The analysis procedures presented include two computer program
packages known as FEMESH and ANSYS. An anchored pavement section of
known geometry is chosen, and its behavior is evaluated by sets of
mechanistic models which have been computer programed.
A subbase and a subgrade material system of known properties are
also evaluated.
Figure 1.1 shows an interface connection between a finite pavement
element and a finite soil element. Those interface elements transmit
compression forces, but they don't take any tension forces (that is,
disconnect in tension).
The manual is composed of six chapters and three appendices.
1 . INTRODUCTION
2. ANALYSIS PROCEDURE
3. OPERATING INSTRUCTIONS FOR FEMESH
4. OPERATING INSTRUCTIONS FOR ANSYS
5. ELEMENT LIBRARY FOR ANSYS
6. CONCLUSION
APPENDIX A  NOTATIONS
APPENDIX B  THEORETICAL BACKGROUND FOR ANALYSIS METHODS
APPENDIX C  THEORETICAL BACKGROUND FOR ELEMENT LIBRARY
Each chapter has been organized to provide the user a procedure in
order to collect the necessary data and run the program ANSYS. Chapter
2 and 3 describe the necessary steps for computer familiarization and
data collection. Chapter 4, the user's guide for ANSYS, has been written
so that it can be used independently by the computer analyst. Chapter 5
outlines the elements recommended to be used in ANSYS.
1.3 RELATED DOCUMENTS
The manual is developed with the intent of minimizing the amount
of reference to other materials. However, references 7 and 8 should
be consulted if preprocessing or postprocessing routines are desired.
interface element
f = NODE OF ELEMENT
a) Twodimensional Elements
interface element
• = NODE OF ELEMENT
b) Threedimensional Elements
Figure 1.1 Soil Structure Interface Connection
CHAPTER 2
ANALYSIS PROCEDURE
2.1 COMPUTER CODES USED
The software used to conduct the analytical investigation in
cluded two programs  one for mesh generation (elements and nodes)
with the name FEMESH and one for the actual analysis called ANSYS.
The former was written as a general mesh generator with several
criteria in mind: ease of use, minimization of input data required,
and ability to generate any two or three dimensional rectangular
mesh of arbitrary number and spacing of nodes in the x, y, and z
directions (Fig. 2.1). Format for the output of nodal coordinates
and element data is consistent with either ANSYS (Engineering ANalysis
SYS t ern developed by Swanson) or SAP4 (Structural Analysis Program
developed at Berkeley).
ANSYS is a proprietary general used, large scale, finite element
code with great versatility. Static, heat transfer (steady state and
transient), dynamic (modal, forced vibration), electrical, and non
linear (geometric, elastoplastic material, creep) analyses are
possible using a large scale element library (a variety of more than
60 elements) comprised of two and three dimensional elements.
2.2 PREPARATION OF COMPUTER INPUT
The computer input consists of the system control cards and the
ANSYS data deck as shown in Fig. 2.2. The Cyber 176 System shown in
Fig. 2.3 was used' in connection with the work at I. LI.
2.2.1 System Control Cards
The first card of an input file is interpreted as a NOSBE jobcard
and must be of the following format:
XXXXX, PARAMETER STRING. CHARGE, USERNAME COMMENTS
Where XXXXX Job name, must begin with a letter. Other
characters may be alphanumeric. Names longer than
5 characters will be truncated to 5. Jobs submitted
through INTERCOM have only the first 3 characters
preserved.
All of the following parameters are optional, and have default values
if not specified. Parameters may be in any order and are separated
by commas.
TU N is a decimal value for CP Time Limit in seconds.
Default is 10.
CMFL Ft is the maximum field length in octal words
required by the job. It is recommended that if
the default Fl is sufficient to process all steps
within a job, the CMFL parameter be omitted from
the joo card. See SYSTEM DEFAULT VALUES AND
LIMITS for the default CMFL allocated to each
job.
ECFL FL is the maximum large core field length in octal
TK word blocks required by the job.
PJ J_ is the requested priority value and ranges from
1 to 5, Default is 4,
MTN N. is the number of 7 track tape drives reserved
by the job.
PEL
or L is the number of 9 track 1600BPI tape drives
NTL that will be required by the job.
HDL L is the number of 9 track 8Q0BPI tape drives
that will be required by the job.
GEL L is the number of 9 track 6250BPI tape drives
that will be required by the job.
DYYMM YY is the dependency string identifier and
MM is the dependency count.
The charge number is a "six digit (leading zeros must be present)
account number, OPTIONALLY followed by a 1 to 3 character suffix
for extended accounting . The extended accounting is used for sort
ing when the Billing detail of run is provided monthly. The user
name is given as a "Last Name, Initials." The initials are one or
two of your choice as specified at account initialization and entered
into the System Access Authorization Table. Any difference between
the jobcard entry and the table entry will cause the job to abort.
Note that blanks are suppressed when scanning the jobcard, so if
only one initial is used, it must be followed by a comma if subse
quent comments are placed on the jobcard. If it is not, the first
character of the comment will be picked up as a second initial, and
job abort will occur.
EXAMPLES
RUNID,T10,P4.264786ABC,MILT0N,JE. Test Run
RUNID,T10,P4. 264786, MILTON, JE. Comment  No Extended
Accounting
RUNID,n0,P4.264786,MILT0N,J, If previously set up
with one initial
The rest of the control cards to call the 2nd revision of ANSYS are
as follows:
ATTACH(TAPE22,R2ANSYS)
C0PYBR(TAPE22,ANSF7)
C0PYBR( INPUT, DATA)
ANSET(DATA)
FILE,TAPEn,8T=C,RT=w",MBL=5120,F0=Sq,SPR=YES,USE.
RFl(XXXXXX) (XXXXXX MUST 3E AT LEAST 170000' OCTAL WDS)
LDSET(PRESET=ZERO,.MAP=S/ANSMAP ,STAT=TAPE1 1 )
SATISFY, BAMLIB.
TAPE20(DATA)
7/8/9
(ANSYS DATA)
7/8/9
6/7/8/9
For big jobs, including threedimensional elements, it is advised that
the 3rd revision/extended core version of ANSYS is used. The control
cards for the above revision of ANSYS are as follows:
JOBCD, — ,ECXXX. (XXX NUMBER OF 1000 OCTAL WD ECS BLOCKS REQD)
ATTACH, A, R3ANSYSECS.
LIBRARY A.
RFl(XXXXXX) (XXXXXX MUST BE AT LEAST 170000 OCTAL WDS)
FILE, TAPE! 1 ,BT=C,RT=W,MBL=5120,F0=SQ,SPR=YES, USE.
ANSYS.
7/8/9
(ANSYS DATA)
7/8/9
6/7/8/9
2.2.2 ANSYS Problem
ANSYS input data is set up in a relatively simple fashion that
makes learning the code quick and easy. Sequential sets of cards are
lettered "A" through "S", "A" being the title card, "S" being a ter
minator.
For example, a previous run of FEMESH to generate nodes and elements
would supply "F" and "E" cards, respectively. The general purpose of
each card group when applied to heat transfer or stress analysis is as
follows:
A  Title
B  Accounting and core aize
C  Analysis options (control)
D  Element data (types, miscellaneous properties)
E  Elements
F  Modes
H  Material properties
L  Load control
M  Load control
N  Specified displacements (specified temperatures
for thermal analysis)
 Specified forces (specified heat flow rate for
thermal analysis)
P  Specified pressures (specified convection for
thermal analysis)
Q  Temperatures (heat generation rate for thermal
analysis)
S  Terminator
2.2.3 LoqinLoaout Procsdures for Batch Users
Every BATCH user has a USERNAME and PASSWORD which allows access
to the CYBER 176 computer facility.
BATCH USERS
1. Dial access Number for desired baud rate:
2. When connection is established, set data phone to "DATA" and then
replace hand set.
3. System will respond with:
ITEL CONTROL DATA INTERCOM 4.
DATE MM/DO/YY
TIME HH. MM. SS
PLEASE LOGIN
4. You type and send:
LOGIN, USERNAME, PASSWORD
5. System will respond with:
Date LOGGED IN AT Time
WITH USED ID
EQUIP/PORT
6. Hit Carriage Return (CR) and system will respond with:
LOGIN CREATED Date
TODAY IS Date
IMPORTANT SYSTEM INFORMATION MESSAGE....
COMMAND
7. You are now ready to send and receive BATCH commands and messages.
In particular, you can now read in card decks and print output from
previously run jobs.
8. To submit a 3ATCH job to the system, place the card deck In the
reader, mal'e the reader ready, and" type "R" . The deck will then
be read into the system.
a. mi uer cne iait wra or zne dec.< nas oeen successfully read, the
system will once again respond with:
COMMAND
TO. When a job is ready for printing, ready the printer and type
"ON, LP" . ATI jobs waiting in the output queue will then print
until the queue is empty. The terminal will then return to
COMMAND mode.
11. To disconnect the terminal from the system, type and send:
LOGOUT
12. Restore dataset to "TALK" position; lift phone to check for dial
tone and then replace handset.
NOTE : This ensures that the phone is properly disconnected.
NOTE : The SUP parameter is optional and can be used on the LOGIN
command (Step 4): LOGIN .USERNAME, PASSWORD, SUP. The use
of the S]1P parameter would result in the elimination of
Step 5.
2.2.4 Remote B s tch Terminal Commands
All BATCH terminal commands are documented in the INTERCOM V.4
Reference manua* .
COMMAND
H.I
H,E
H,0
FILES
WAIT, LP
GO, LP
C
R
EVICT, 
DESCRIPTION
Displays your jobs in CYBER 176 input queue
Displays your jobs in CYBER 176 execution queue
Displays your jobs in Cyber 176 output queue
Displays all jobs at your jobsite and the queue
they are currently in
Suspends job currently printing
Continues a suspended print job
Resumes interrupted operation
Read cards
(Last 2 letters of job name) Drop job from input/
output queue before printing
E,LP
ON, LP
RFW
BSP,LP,N
RTN,,P
M,msg
REP,,N
PRIOR, — ,
STATUS, —
STATUS,,—
Kills job while printing
Turns line printer logically ON
Rewinds current output file
Backspace N of output file sectors
Halts printing and returns job to output
queue with priority P
Send message to central site
Job is reprinted N additional times
(Last 2 characters of output file and then
priority you want to raise it to).
Status of job (from your siteID) whose 1st 3
jobname characters are — .
Status of all jobs from site ID.
2.3 ANALYSIS METHODS
This section is intended to give a brief summary of the methods
used in the various types of analysis. It is not intended to be a
complete theoretical manual or to answer all questions which may arise
on the theory behind the ANSYS program. Such detail would expand the
already voluminous User's Manual and is better included in a Theoretical
Manual. Theoretical details may be obtained by contacting Swanson
Analysis Systems, Inc.
Figure 2.4 gives a summary of the ANSYS Analy sis types available
and may be used as a guide in selecting which type to use.
2.3.1 Static Analysis
■ In the matrix displacement method of analysis based upon finite
element idealization, the structure being analyzed must be approximated
as an assembly of discrete structural elements connected at a finite
number of points (called nodal points). If the forcedisplacement
relationship for each of these discrete structural elements is known
(the element "stiffness matrix") then the forcedisplacement relation
ship for the entire structure can be assembled using standard matrix
methods.
The general form of the equilibrium equations for each element is:
CK.I «,}  {F,} (2J)
where, [K ] is the element stiffness matrix
{U } is a vector of the element nodal
e displacements, and
{FA is a vector of the element nodal forces.
e
For the total structure:
[Kl {U} = {F}
where, [K] is the total structure stiffness matrix
(2.2)
X [KJ
11 a
{11} is a vector of all the nodal displacements in
the structure
{F} is a vector of all the corresponding nodal
forces, thermal forces, and pressure forces
11 e
If sufficient boundary conditions are specified on (U} to guaran
tee a unique solution, equation 2.2 can be solved to obtain the nodal
point displacements at each node in the structure. From these dis
placements the forces and stresses within each structural element can
be calculated.
For plasticity and creep problems an incremental technique is used.
The loading is applied in increments and at each loading level an elastic
solution is done, with a correction applied to the next loading step to
account for the plasticity and creep occurring during this loading step.
In this procedure, the plasticity lags 3 the loading and the calculated
stresses are somewhat higher than the true stresses. The amount of
this conservative difference can be reduced by increasing the number of
load increments or by running iterations with no increase in loading to
refine the solution. Unloading and reversed loading can be handled
with no difficulty by this technique. The von Mises yield surface is
used, along with the PrandtlReuss flow relations. The stressstrain
curve upon reversed loading is assumed to be the same shape as the vir
gin stressstrain curve, but offset to account for the strain due to
previous plastic deformation. Kinematic or isotropic hardening rules
are also available for the treatment of cyclic plasticity.
The program will handle creep by a similar incremental technique.
Both, primary and secondary creep equations are available to the user.
The user has the option of selecting either a creep formulation which
assumes the stresses decay due to the creep (as in thermal stresses),
or a formulation in which the stresses are independent of creep (as
in primary stresses).
The ANSYS program also includes irradiation induced swelling and
creep for use in the analysis of nuclear reactor internals. The swell
ing is not stress dependent and is treated in a manner similar to
thermal strains, while the irradiation creep is a stress and temperature
dependent pheonomenon and requires an iterative solution.
For large deflection analysis the geometry is modified at the end
of each load increment so that the total loading is applied to the
deformed structure at the next load increment. This procedure thus
follows the large deflection loaddeflection curve.
If the load is applied to the structure in a single step and the
rate of convergence to the large deflection is observed, an estimate
of the stability of the structure can be made. In particular, if the
deflection diverges, the load is above the critical buckling load.
This large deflection analysis then becomes a stability check.
The basic equations for the formation of the element equilibrium
equations are summarized in Table 2.1. The same definitions used here
apply to all other analysis types except the heat transfer analysis.
2.3.2 Heat Transfer
Transient and steady state heat transfer problems can be solved by
finite element techniques analogous to those used for structural
analyses. In this case the basic equilibrium equation is:
[TUT} + [K]{T} = {Q} (2.3)
where, [K] is the thermal conductivity matrix
{Q} is the heat flow vector
{T} is the vector of the nodal point temperatures
[Cl is the specific heat matrix
This aquation is identical to the nonlinear dynamic equation
except that the mass term does not exist. The solution technique is
the same as for the dynamic analysis except that linear and quadratic
options are available for this approximation function.
This equation is solved in ANSYS at each time point in the heat
transfer transient. Material properties (and convection coefficients)
can be a function of temperature. In a steadystate analysis the pro
perties are evaluated at the temperature of the previous iteration.
In a transient analysis the properties are evaluated at a temperature
extrapolated from the previously calculated temperatures.
The temperature output from the ANSYS heat transfer analysis is
in the required form for input to the ANSYS stress analysis, giving
an integrated analysis capability.
The basic equations for the formation of the element equilibrium
equations are given in Table 2.2.
2.4 LOAD CHARACTERISTICS
Pavements are subject to axle weight distributions produced by
the traffic volume. Vehicle speed and load duration are not included
10
in this report. The load input consists only of the static weight of
an automobile, and the corresponding pavement response is evaluated.
Static load can be input as nodal forces (See Fig. 2.5) or
element surface pressures. Environmental loads, however, cause more
damage to the pavement. Moisture variation is handled by varying the
modulus of elasticity of the top four feet of the subgrade soil (of
course the variation of modulus with moisture content must be known
as an input) .
Temperature variation in a time domain can be input in a heat
transfer model as shown in Fig. 2.6. The resulting temperature dis
tribution can be handled as a thermal load for a static analysis.
2.5 MATERIAL CHARACTERIZATION
All material properties are listed in Table 2.3. Table 2 A
represents the material properties needed for the element library
used in this report.
11
TABLE 2.1 SQUIL13RIUM...EQUATTGNS (Static Analysis)
FOR AN ELEMENT
C;< a ]{u 3 > = {? a }  {Q e } + {R a } + (s e >
wnara
also
DO  CT3] T [H] T f [g] T [C][g] dV [H] [TR]
e J V
{U a } s Nodal displacement vector (in global coordinates)
(? a > = Applied nodal load vector
{QJ ■ [TRj'CH]' f [gl T [C]{£.„ > dV = Thermal load vector
e j y in
{RJ s [TR]'[H]' f [e] T {P} dA = Pressure load vector
6 JA
{S }  [fO{AJ s Body force vector
e e c
{U} = [TR]{U } = [H" 1 ]Cb> = Nodal displacement vector
in local coordinates
[TR] s Geometrical transformation matrix
[U] s Matrix relating the nodal displacement vector in
local coordinates to the displacement function
{b} s Vector of the coefficients of the displacement
functions
{w}. = [e] {b} = Displacement functions
[e] = Matrix of displacement shapes
Ce} " Cg3"Ch> = elastic strain vector
it* } = Thermal strain vector
[g] = Matrix relating the elastic strains to the displacement
functions
[C] = Elastic material property matrix
M = [C](U>  ^[ n H ' stress vector
{?} = Distributed load vector
[Ml '=CTR] T [H] T f p [e][e] T dV [H][TR]
p = Density
(A }  Acceleration vector
c
12
TABLE 2.2. EQUILIBRIUM EQUATIONS (Thermal Analysis)
rQiR AN ELEMENT
CC e ]{7 e }  n< e ]{T a } = {Q e }
wnere,
CCJ = [H] T /" P CfeKe} 1 dV [H] = Spec"
tic neat matrix
{T a } = Vector of time derivatives of nodal temperatures
[KJ = [H] T f [g] T [!<j[g] dV [H]  [H] T h{e}{e} T dA [H]
J V S
■= conductivity matrix
(T } = [H~ ]{b^} = Vector of nodal temperatures
(Q a ) = [H] 1 J p q{e} dV + [H] 1 7 h (a; dA = Element heat
V S flow and heat
generation
vector
.lso,
{b.} = Coefficients of temoeture functions
z
§  = {e} 1 {b*} = Temperature distribution over the element
X I L
{a} = Vector of temperature distribution shapes
p = Density
C = Soecific heat
P
{$  .} = [g.,.]{b.} = Vector of thermal gradients
[3*] = Matrix relating the thermal gradients to the
temperature functions
[k] = Conductivity material property matrix
q = Internal heat generation raze per unit mass
T = Coolant temperature
c
h = Convection coefficient
13
TABLE 2.3 MATERIAL PROPERTY NAMES
Property
EX
EY
EZ
ALPX
ALPY
ALPZ
NUXY
NUYZ
NUXZ
DENS
*C
*KXX
*KYY
*KZZ
*HF
*VISC
Units
DescriDtion
Force/Area
Force/Area
Force/Area
Strain/Temp
Strain /Temp
Strain/Temp
Mass/Vol
Heat/Mass*Oegree
Heat
* Lenqth
Time 3
'Area^Oegree
Heat
* Lenqth
nme :
*Area*Oegree
Heat
* Lenqth
Time :
*Area*Oegree
Heat
Time 3
*Area*Oegree
Force * Time
Length'
nu
— *•«*
GXY
Force/Area
GYZ
Force/Area
GXZ
Force/Area
DAMP
*0HMS
Resistance*Area
Length
*EMIS
— — .
Elastic modulus, X direction
Elastic modulus, Y direction
Elastic modulus, Z direction
Coefficient of thermal expansion,
X direction
Coefficient of thermal expansion,
Y direction
Coefficient of thermal expansion,
Z direction
Poisson's ratio (X strain due to Y stress)
Poisson's ratio (Y strain due to z stress)
Poisson's ratio (X strain due to Z stress)
Mass density
Specific heat
Thermal conductivity, X direction
Thermal conductivity, Y direction
Thermal conductivity, Z direction
Convection or film coefficient
Viscosity
Coefficient of friction
Shear modulus, XY direction
Shear modulus, YZ direction
Shear modulus, XZ direction
K matrix multiplier for damping
Electrical resistivity
Emissivity
* Used only for the Thermal analysis (K201)
14
TABLE 2.4 MATERIAL PROPERTIES VERSUS ELEMENT SUBROUTINE
Element Subroutine
Material Property
STIF<12
OR
STTF45
EX
NUXY
ALPX
DENS
STIF12
OR
STIF52
MU
STIF55
C
/vv
<YY
DENS
STIF32
C
KXX
DENS
15
y
>■
a) Twodimensional Mesh
y
— < —
b) Threedimensional Mesh
Figure 2.1 Arbitrary Rectangular Mesh Generation
16
ANSYS PROBLEM
(A  S)
/
£.
739 MULTIPUNCH
(COLUMN 1) CARD
SYSTEM CONTROL
CARDS
5789 MULTIPUNCH
(COLUMN 1) CARD
789 MULTIPUNCH CARD
(COLUMN 1)
hese two cards separate
the problem from other
cards.
Figure 2.2 ANSYS Setup Deck For CDC Computer
17
524 <
LCME
SmNOED
MEMORY
Figure 2.3 Cuber 176 Configuration
13
TRANSIENT AND
STEADY STATE
THERMAL ANALYSIS
(K201)*
STATIC ANALYSIS,
LINEAR AND
NONLINEAR
(K20=0)
NONLINEAR
TRANSIENT DYNAMIC
ANALYSIS
(K20=4)
REDUCED LINEAR
DYNAMIC TRANSIENT
ANALYSIS
K20=5)
HARMONIC RESPONSE
ANALYSIS
(K20=3)
REDUCED HARMONIC
RESPONSE ANALYSIS
(K20=6)
MODEFREQUENCY
ANALYSIS
(K20=2)
* ,<20 is the key input on the CI card to select the analysis type.
Figure 2.4 Suircnary of ANSYS Analysis Types
19
TJ
TJ O
U~T7
NLl
1 NL3
Nt2
LD1
NL4
> i ' e
a) Truck Model
LD2
b) Passenger Auto Model
NL  Static Load on Node of Mesh
LD = Longitudinal Dimension of Automobile
TD = Transverse Dimension of Automobile
1 NL5
9
NL6
Figure 2.5 Static Load Model (Dimensions and Load Will Vary With Vehicle)
20
UJ
TIME
STAR"
RESTART
Figure 2.6 Temperature Load Model (actual values have been
explained in the example problem discussed in Volume
3 of this series of reports entitled: Anchored Pave
ment System Designed for Edens Expressway )
21
CHAPTER 3
OPERATING INSTRUCTIONS FOR FEMESH
3.1 FEMESH SOURCE CODE
FEMESH was written with the specific intent of generating rectan
gular meshes for analysis of pavement systems. Provisions for including
layers of varying materials is made. Output is available in SAP4 or
ANSYS format, either as a punched card or directly written to a tape or
mass storage file for use when the analysis is initiated (after data
decks ) .
3.2 INPUT DATA
The following
are the
input formats
for FEMESH data:
Card
No. Column
Format
Variable
Description
1 130
2QA4
TITLE
Job Title
2 15
15
NOPT
LT.Q generate nodes only
3 610
15
N
Number of first node
(useful when punching
different meshes for
assembly in ANSYS)
15 15 FORM Output format
.IE. ANSYS
.GT. SAP4
1115 15 NX No. of nodes in xdi recti on
1620 15 NY No. of nodes in ydi recti on
2125 15 NZ No. of nodes in zdirection
2630 15 NPUNCH .GT. Punched & Printed
.IE. Printed only
180 1615 MAT Material number
180 8F10.0 XP xcoordinates of nodal lines
180 8F10.0 YP ycoordinates of nodal lines
180 8F1Q.0 1? zcoordi nates of nodal lines
Blank card
Note: Cards 5, 6, and 7 should be input in increasing order. Use as
many 4, 5, 6, and 7 cards as necessary.
The listing of the program FEMESH is shown on the following pages
(pages 23 through 29).
22
I I
I >
X
LU
s.
O
S
Q
O
CD
4>
00
*l
21
2i2
3 3
_ ;
zi
—
Cf
""W .1
VU
V* —
UJ •="
>" u.
2^ «
W
CI •«
2T. 'j.
ZJvi
•< C
■J _J
2li. <
— • "< —
! vi <
d .5
; •  a
j — :  OiS
ti 2
31 3 3
is — Z
— S U. I 2
u: o «J 'j 'JUUU'Jig
o .—• a =»• 2
r 3 J. ^
! jo
! U 2 3
i a 52 o
; i 2 i _ 
i>us = ;
x  "" a
vl _ —
■ ■/ u ' J 
: 3 G 2 •<
*. w u) O 2
c >. vj a i
; ■* —
i >■ <j
S • U. < J
s o o a =
. 2 • >• «e 3 i
2
^ (J •
2 2 •
 3 —
X Si <
2 2 2
 !
U
3 I
(J
i. 2
2 a
O 2
= — 2
UJ vi
13 2
— 2
— 3
^* ; —
x * .2
— x
• — — J '—I
2 •< 3 _l _i
2 2 T — —
i. O
2 X
Z
2 •< — «a
U 3 IM fl»
— 3 —
2 *» • 
2 x >» "*4 —
> 2 Z Z
— • 1 1
1 1 i
— 2 U
 J I
■v. . I
2 IN
2
2 —
2 I ■
2 a.
ij —
.rt .> >.
3 2 —
•< < 2
V/l —
= 3
_. _i : — _ 'a
.1 vll 2 » 2
« « — 3
— ^J 'o '_ 'J ^ SJ J U
2 >
» 2 >
> — •>
> 2 »
■>  •>
■> _i >
■> 2 •>
> 3 >
* 2 >
I sJU U UU
■> * >
«•»»•■>
>
>
>
>
•>' ■>
>
^.
:
n
—
%i
J" "»
J
F*
^z
^j
■j
1M
«J .Vi
."M
•J
m
3 •> ■>» *
m .l r; d
<3 >■ 3 C> 2
23
C
4>
C
o
o
oo
13
i
cn
o
s_
Q
O)
cn
4>
IS)
IN* »
 2 »« >» .Nt
> >• 2 2 2
a 2   
x • 1 1 I II I I
2
3 O — •* >• **
2 U. «S — — —
2
3 o r 3 <. 3
r* 2
i ii ii
— ~5
i
J
1
1
M
•
1
i
•
~m
1 
1
2
* .1
•
— ?M
^
>j

(^
•
— 3
;
^
— —
a
»
—
—
,
x
— 3
!
•
o J
a
J
3
2
<
— —
,
.J
• — *
.—•
<j*
2
3
2
— *
Z •
3

_l
«
— •
<J
— 2
*
»
3
2 «
1
■<
■«»
C
1
S
3
<"^ 2
J
2
 <j
r
2
a
i 2
2
*j
w
— 3
— 2
2 t ■>
2 i* 2
2 2 2
uj ■— 1 i U* — * J C 21 2 2 — — — '<*4
J< ^ >4 i.
ii i i u vw •*»
X >• ^* — vl
I *
■u 2 J C
>
•>
[
; ■>
'
>
f
{
>

_i
>
>
>»
* ■>
>
>
» O
a
>
>
■ 3
_
*NI
.%
■>
: .%*
*
>
!
>
1 o

a
^
*
>
; —
^
2
•
?
>
■
—
X
■>
>
i 2
2,
3<
— ■

>
z
■>
; 2
C

— •
2
■3»
2
>
M
2
2
! ■>
—
■>
• —*
»•
2
•
>
—
>
i 2
<
J
—
•>
<■
.y
'
21
: —
2
2
•»
2;
>
•
UJ
2
•
2
>
«j
■z
1 **•
2
, 2
n
1
•>
2
>
 —
—
' ■»!
2

1
>
—
■>
j «
J

U
2

•>
J
>
1
1 3
2
m
.J
'•J
■2
>
! *
*^
 ■—
2
—
2
2
. >
—
■>
* i.
2:
I
CI
2
2
J
2
■>
1 3
■ji
i '— *
2
'_!
—
^
>
_j
>
^
•>
2
>
—
2
■>
—
>
1
2
1 2
4»
:;
■c
2
>
_j
>
'■ '*.
<
a
~*
3
u
*J
>
■>
—
•>
I — i
' 2
T
2
>
•
>
,
C_l l.
1 .M
c\l
J L;
LJ
>
•>
i
J
> >
■J •> ■>
J •
> 9 * * * : J > ? > ■■> > •» >
■vi j r» a s» 2 — "i r* s: t 2 •—
.1 *1 U1 .T ."J 2 J J J J J 3 J
J J» 2 —
J J f— .—
1 J T J .— 3 T* 3 — >i
24
! I
■a
Z5
C
! a
c
o
(J
03
S_
O
s_
en
c
» —
2 2 >•
•a 3 ;
3
~5 : ~3
) i —
. 2 —
i — a 
■— i 2 3> 2
21 2 21 I
— o  2:: s z:
_ a — — o —
3 — . j — i — . o —
— r r r
• • 2 2 2
or . . .
i • 1 1 1 1 i ■
^4  ~i —
2 **■*
•2323
— . — .n n i^l
vi u. 3 3 2
2 — <M
• 22
>• 2 2
— • It II IE
2 1 C* ~1
Ui — — —
n 2 2 2
1
2 2
1 1 u ~
J .1 J p 3 '__
2 2 2
2 2 2
vi J 2 — 24
2 S_
i iu 2 — O
U3; j
•■d _4 _  <_) ij CI (J 3_
vit • O 2 — 2— '2— • ■_* — • ul
_J 3 wJ 2 _) — — —
2: «■* s'j.sa ;
<l u — jl — 31 O 2
=: 3
— .j
j _< —
3 3 i
> > >
24 ■> X >
I— 3 ■> 2
>t J •>• > ■>• > >l
V ■■> •>; > •>'
■3 r* 2 — ^i
25
a
CD
3
c
c
o
u
2r
3
i. VI I
2 s
I !
3
a — —
cvo
S V N VI J
<t3
i_
CD
o
0)
— . (M 
>• 2 32 j
VI .1 .1 'J1    — ~
en
C
■M
CO
5
IN O 21 3
3 o
z
v> —
O 3
r^ 3 — — X X
■< 3 3 O <N i — _ I —
— 'J U U  <vj .i — . 'j. —
3 X > \ . X » — CM ■•n »3
3 3 3 3  • x >n > x ji .  _
HZ—  — — fl XII
<1 ui »i ji x '.l »i ii   »s — o 
..... .—— m  *o «— ■
WX>C5<~>» M X. X — — ' J1 —• 3
a a
a —
3. 3 o a a
<S <ii ^ <z
r r r r
3333333333
—• i">4 "I J
^» .1 O 3
3 "i •=■ ji 3 ?i
3" n r ci r> r>
3 "J 3 ^J
J A4 — i — I
•> > •>
>■■ >
3 —
> > > >t ■>
3 > > x :•
r» 3 — "J ■■">
si st 3 . 3^3
* *
25
jl
I i '
i .
li
i I
i ■>
a
3
O
u
on
I
=
ra
S
cn
o
i.
Q_
sz
I >
c
I > =
 •> — •>
— i > x •> : —
3
a
ii I li 1 1 Zt
— • <>» *i :r Jl >3 3
> 4 > . _
■< < <«•«:■<< ■_!
   = ^ ■— i
27
c
o
u
I I
I I
m
E
<T3
S_
O
s_
Q_
O)
JZ
4>
en
u.
I ■» z >
c
— •
!■*«■>
1 —

1 » — •>
4>
■j
!•>—:•
00
3
;•»—•>
—
» a ■>
1 ■> z *
> a >
1
3
J 3
x 3 ^
.r 3 _s
3
x ^ ivt
• 3 > 3 2 , a j 3
> 3 ■> 3 . u U U
3 * O > W Wl M I b 1 1 I I I t Ml
O > 3 > J 2 — — — — — — x;.V4
•> t Ui i_l •— fM ■T .» fl d — — —
>C> — 3 — — — — — .—
»^.> — 3333333——"
2 M 2 II i«ii 2 ii «
— O _i <J <! <J —I U _ 2
— I .vi
.I I
O u u y u
■>>•>*> m * a
^;^i ; r =j ^. c — c;
coo— a
■ a .— =;
28
C
+>
c
o
Li.
E
s_
ai
o
s_
en
c
«•
>
_
•>
M
UJ
■>
■<
£
Z
—
■>
•>

1
a]
>
—
3S
—
Z
>
~
•}*
;
Z
—
•>
.u
■>
T
Z
?»
s
»
[
—
• !
X
•>
—i
>
!
—
J
•Si
_t
>
i
—
C
uI
•J
UJ
•>
o
Z
MM
*
■>
—
**i
!
Z
■>i
u
>
•<
«tl
•>
l/l
>
z
^
!
uj
■3"
—
•>
Z
—
z
■>
£
■>
.
.2
XJ
—
—
>
•>
a
_l
I
i
mm
•X
"1
■>
2:
n
^*
—
«M
>■
Z
*
~
X
UJ
VI
z
■ i
in
Z
a
•>
vl
•>
,3
zz
»
—
—
1 1
c;
•>
:•■
■>
UJ
—
a
—
(VI
—
s
•X
1/1
£1
■—
r
z
—
—
'Z.
3
•>
2
•>
Z
—
ct
•<
s
:»•
vi
■~l
■«
v4
—
s
_«
z
Z
2
—I — »l — ■<
I II
—J 3
<i a
z: j
U <J !_l 'J <_i
i J <—> a I*' 3 — <m
j ..I ,3 .— . a 7> c
29
3.3 MESH GENERATION EXAMPLE
To use FEMESH, consider the example shown in Figure 3.1. All that
is necessary is to enter the number of nodes in the x, y, and z directions,
and the coordinates of the nodal lines in the x, y, and z directions, re
spectively. An example of the input is show below on the FORTRAN coding
form.
An Example of a FORTRAN Coding Form for FEMESH
ISM
fanTAAM C*i, M Fun
GX237327 4U/U050**
—
FEMESH
I 1 .
1 1

11 1 1
■*>■■■■—«
S.G.MILI7S0P0UL0S
104/04/79 ! ™ 1 —
i 1
I
ii>d<ii<ijo «••>••
J — r I
'Omi«i WaUm*m1
s=a
MEjSH i G
rrt
.ld
1 1
FN£RAm 1 ON
m
1 1
^2
GO.
eco
1 1
i '4
i I i S
TOT
fTEST i ilPH INnTC
I I
Ml I
200'
"S CO"
i mt nrn
□TTI"
PIT
I I l
MM
Tilt
J3QCJ.
_6co;
i i
imii
1 1
nr
MU
310
I i
I ! I
i i M LLMi
I I
ML
I I I ! I I ill
I I I
I I
I !
! I I
i I II I
! I
! i I
rm
! !
TT
Mill
! ! ! I i
i M ! i I I
TTT
i n ! 1 1 1
I I
1 1
1 1 i
i III
I I
ill
I I
I I
I I
I I i
~rn
MM
I I I
i — r
l i
TT
TTI'
jrrr
TTT
1 1
! ; i
i i ■ i
i I
TH"
1TTT
i I
LlA
Mil
! I
I i !
I I
i I
I I I I
T
"Hr
IMT
1 : TT
TT~_i
lift
i ! I
im
TT
! r; 1 1
Mil!
! : i m
! ! i !
mi
30
. Q
100. 50. 0.
C_) = Node Number
/ \ = Element Number
Hll\ 72 NODES
*£«/ 30 ELEMENTS
The uncircled numbers indicate the dimensions of the
mesh in inches.
Figure 3.1 Example of Mesh. Generation
31
"he output of the example proolam using FHflESfl is as follows
Output of Example Problem Using FEMESH
3—3 M £ S H GENERATION T £ S T ( ? S I N T £ Q N L Y
NOP
LT G NC0E5 ONLY
Fjfii'U
1 G£ Q SiP<+
L T Q a ^ S Y S
NUMSES CF NOOES 1Z
MY
NZ
« A T iLSJAL v ' u H c  £ 3 Q " <  y £ 5 S ( go I T.C m t o to ?)
1112 3
,..C £0 >,g
.aaa
i a a . a a a
.ggo
■Z. CO a a □
1CG.GCG 2GG.GGQ 5GG.QGG 31G.GGC 32G.CQG
.GGG 2CG.GGG 4CG.GGG 6GC.GCG
32
Output of Example Problem Using FEMESH
NOOE generation results
1
nnnp
.nnnn
p n n p
2
.CGGO
I G U . G C G G
.QGGC
3
n n n n
7 p p . r, n n n
. c a, n n
4
► GGGG
iGG. GGGG
.GGGG
*
.nnn p
7 i p . n r. n n
. nnn
6
,ccaa
32G.aCGG
.GGGG
7
 r
. r p r, n
. q p p n
. p P p p
5
5G
.GGGG
1GC.GGGG
• GGGG
Q
5 G
. n G G
2PC.QGG0
• GGGG
1G
SC
.GGQG
3 Q G . G C C G
.GGOG
i i
5 G
. n n n n
71 n. anna
.nnnn
12
5C
.GGGG
32G.GGGG
.GGQG
i ?
i nn
.rrqn
. nc^ n
,nn^n
14
1GG
.GOOG
iac .acac
.coaa
1 5
i no
.nnnn
? p p .nnnn
.nnnn
16
ica
►GGGG'
3GG.G0G0
.GGGG
1 7
i nn
. nrinn
"in.nnnn
. n a a a
IS
iaa
.GGGG
32G.GGGQ
.GGGG
1 o
. rinnn
.nrnr
? n p . p. p p n
2G
.GGOG
1CG.GCCG
2GG.GGGG
2 1
. GGGG
2 G G . a C G G •
2GG .GGGG
22
,GOGC
3GC.GC00
2GC.GGGG
77
.nana
7 1 g . a g a g
2 a a . g a g a
24
.GGGG
32G.GQCG
2aa.GGGC
75
5 f!
. n n n n
.nnnn
?r^.nn P P
26
50
.gogg
IGG .GGGG
2QG.GGQC.
27
sa
.GGGG
2GG.GCGG
ZSCQCGG
23
5C
.GCGG
3CG .GGGG
2QG.GGaa
29
5G
.nncG
3 1G.GGGG
2 G a . G G U C
3Q
5G
.GaaG
32G.CGQG
2aa.aaGG
31
iaa
.GGGG
.GGGG
2GG.GGGC
32
iGG
.GOGG
IGG. GGQG
2 G a . C G G ;
33
1GC
.GQGC
2GG..QCGG
2 a G . G G G G "
33
Output of Example Problem Using FEMESH
34
1GG«
GCOO
3GG,
.OGGO
2 G G . o o a
35
LOG',
a ooo
3 1G
, G
2 c g . a a g c
36
IGG.
gcog
32G
,GGCO
200.0000
37
GOOG
.caac
i o a . c a a a
33
CGQO
IGG
.0000
400 . GGGO
39
coaa
2GG
.GGOG
4GC . GOOG
40
GCGG
3GG
.cccc
4CC. GOOG
U 1
f .1 f* n
Li u u U
3 10
.GGGC
^00.0000
42
GGGO
3 20
.GGGC
400. GCGG
4 3
f' Vt '
GGGC
.OCCC
40G..0aG0
44
50.
aacc
IGG
,OOCC
400.0000
45
5G .
GOOG
2CG
.GCGG
^OG .CCOC
46
5Q.
.uOGC
3GC
.GGOG
4 00.0000
47
5G
i ijGuu
3 1G
.GGGC
.GGGC
4 • . G
43
50.
GCGG
3 20
4CG .CGGG
uQ
LOG
GGCG
. a o c c
arc H o '1 n
50
IGG
.GCGG
IGG
.GGCG
51
IGG
.GGGC
2CG
.0000
. GCGG
u ; ' n n n n h
"* '— >j » U j w Uj
52
IGG
. C G u
3GG
ti n n " "■ n ~
" J tj • ^ ^ L. w
53
IOC .
caaa
31G.
GGOG
400. GOOG
Su
1 HG .
nnnn
3?n
nnnr,
unn.nnnn «
55
GOOG
.aoao
60 0.0000 •
Sft
nnnn
_ LOU
.nnnn
6 0.0000 .
57
GGGO
200
.0000
60G.000C
53
ccoc
3.C_C
► ac.ac
600.0000...
59
aoao
310
.OGGO
6 a c . g a o a
^n
nnnn
3 2.2
.nnnn
600 . nnnn
61
50,
,G000
.oaaa
60Q.G000
A?
sn
nnnn
\ n n
.nnnn
f*nn .nnnn
63
SO
► aaca
2CG
.GOGO
6 o c . a a o a
^a
50
.nnnn
vGG.C
600.0000
65
50
,oaaa
31G
.aocc
600 .GGGO
r> 6
sn
.nnnn
3 7 n
.nnnn
ann.nnnn
67
100.
.caaa
.GGOO
6oa.aaoo
^A
1 nn
.nnnn
i nn
.nnnn
h n n , n n n n
69
1GQ
.oaoc
200
.gooc
6oa.Gooa
7n
i nn
.nnnn
^nn.
.nnnn
^nn.nn n n i
71
100
.oaaa
310
.0000
6 g a . a o o o ;
7?
1 nn
.nnnn
.320.
.nnnn
r,nQ.nnn n '
34
Output of Example Problem Using FEMESH
ELEMENT GENERATION 3E.3U175
I
19
25
7
2
20
26
3
1
i
?
?<<
?i.
a
7
7 '
7 ~
a
i

n
21
27
9
4
22
25
10
1
1
a
a
77
7a
i P
c
7 '
?<3
i i
7
1
p
5
2 3
29
11
6
24
30
12
3
1
a
7
7 c
7 i
1 7
*
7i.
7?
1 u
i
i
p
5
26
32
14
9
27
33
1 5
1
i
a
77
7 7
i P
7 3
* 4
i *
1
i
p
10
23
34
16
11
29
3 5
17
2
1
a
1 i
7 =
7 C
l 7
i 7
7 P
"^
1 2
7
i
n
19
37
4 3
25
2D
33
44
25
1
1
?n
7 3
a u
/ »
7 i
7=s
^ = ,
~ 7
i
i
n
21
39
45
27
22
4
4o
2 5
1
1
G
7?
tip
UA
> 2
7?
4 1
(I 7
7a
7
i
p
23
41
47
29
2^
42
43
^ vj
3
1
a
?p
a 7
uo
7 1
76
ua
n
77
1
1
p
26
44
50
32
27
4 5
51
.13
1
1
^ 7
u =
=; i
7 7
75
u ~
 ?
" !•
1
1
p
23
46
52
34
29
47
53
3 5
2
1
a
7<3
47
S 7
I =
7P
4 =
S 4
62
44
1
1
1
(7
37
55
6 1
4 3
33
56
7A
So
o7
U 4
7G
=;7
o T
4 =;
i
1
n
39
57
63
45
tl o
4 u
53
64
46
T
1
a
UP
t; 3
~ 4
u A
U, 1
c c
o =;
4 7
7
i
p
4 1
59
65
47
42
60
66
43
3
1
u ~
£ 1
o7
49
4 a
o 7
a
= n
i
1
p
44
62
63
50
45
63
69
51
1
1
45
63
69
5 1
Uo
6 4
70
71
 5 2
53
1
2
1
a
46
64
70
52
47
65
a
47
.. 6 .5 .
7!
S3
u*
66
7 7
=; u
3
1
p
35
CHAPTER 4
OPERATING INSTRUCTIONS FOR ANSYS
4.1 WAVE FRONT SOLUTION AND LIMITATIONS
The ANSYS program uses the wave front direct solution method for
the system of simultaneous linear equations which are developed by
the matrix displacement method. The frontal direct solution gives
results of high accuracy in a minimum of computer time.
There is no "band width" limitation in the problem definition .
However, there is a "wave front" restriction . The "wave front"" "
restriction depends on the amount of core storage available for a
given problem . Up to 576 degrees of freedom on the wave front can
be handled in a large core. An optional 1152 wave front is avail
able on very large computers. However, it is recommended not to
exceed the 571 wave front if the CYBER 176 (CDC 7600) computer is
used. The wave front limitation tends to be restrictive only for
the analysis of threedimensional structures or in the use of
ANSYS in small computers. There is no limit on the number of
elements used in a problem, but there is a limit on the number of
elements which consist the wave front. The number of equations
which are active after an element has been processed during the
solution procedure is called the wave front of that point.
For a banded solver, the band width is minimized by paying close
attention to the ordering of the nodes. Alternatively, in the wave
front procedure, the ordering of the element is crucial to minimize
the size of the wave front. A degree of freedom becomes active when
an element containing that degree is processed.
That degree of freedom remains active in core until all elements
containing that degree of freedom have been processed. Therefore,
the element cards must be arranged in such a way, so that the element
for which each nodal point is mentioned first is as close in sequence
to the element for which it is mentioned last.
The wave front must sweep through the model continuously from one
end tcTThe other in the direction wmch has the largest number ot nodT
points . The assembled matrix expands and contracts as nodal points
make their first and last appearance in the element specifications.
The optimum wave front for a simple line element model is a point; for
a twodimensional solid or plate element is a line of nodes; and
for a threedimensional solid, element is an area of nodes.
An estimate of the wave front size can be made by multiplying the
number of nodes in the wave front by the number of degrees of freedom
per node. For example, consider the model shown in Fig. 3.1. The xz
plane has the lesser number of nodes (3x4 = 12). Thus, the elements
should be specified along the upper xz plane in the y direction. The
new ordering of the elements is shown in Fig. 4.1.
36
If the elements described above have three degrees of freedom
per node (say ux, uy, and uz), the maximum wave front size is approxi
mately 12x3 = 36. Often, it is convenient to generate elements with
FEMESH in an order that is not the best for an optimum wave front.
If so, elements may be internally reordered by ANSYS using the Fl cards.
The Fl cards are called into the full ANSYS problem by inputting '
KORDER = 1 (column 78 of the C2 cards). A list of nodal points defining
where the element reordering is to start is input on the first Fl card
set. Additional lists may be defined to allow the user to guide the
wave. The starting list usually consists of one node for a line element
model , a line of nodes for an area element model, or a plane of nodes
for a volume element model. There is a limit of 25 Fl cards or 1000
nodes, whichever comes first. All elements attached to the first node
in the list are defined first, then all elements attached to the second
node are defined next, etc., until all elements attached to all nodes
input on the first Fl card set (but not on later Fl card sets) are
defined.
This procedure is then repeated with the new set of nodal points
brought in with the previously defined elements. If, during the course
of reordering, an element would bring a node that is defined on a later
Fl card set, that element is omitted until later. This feature allows
the user to guide the wave front.
The element reordering, using the Fl cards of the mesh shown in
Fig. 4.1 from the mesh shown in Fig. 3.1 (generated by FEMESH), is
presented in Table 4.2. It is recommended not to use the Fl cards if
interface elements (connecting the slab to the subgrade) are used. It
is rather easier to reorder the elements by hand.
4.2 DATA INPUT INSTRUCTIONS
Abbreviated ANSYS input instructions and the proper formats are
included in this section. Specific quantities to be used for some of
the variables are given in the Element Library (Chapter 5) for the
various element types which to be used. Standard FORTRAN conventions
are used for the input quantities. Variables with first letters from
I to N are integers and must be riant justified (ending in the right
most column) in the specified field . No decimal point should be in
cluded. Variables with other first letters are floating point numbers
and may be placed anywhere in the field. Floating point numbers should
have the decimal point input. The exponent, if any, must be right
justified in the specified field .
No data should be punched on the cards in other than the specified
fields. A blank input is treated as a zero or as a default option
where indicated. Data cards must be in the order defined, and no add
itional cards (except for comment cards) are allowed. Comment cards
may be inserted freely in the data deck. A comment card is identified
by the characters C*** in columns 1 through 4. The remainder of the
card is used for any comment that the user wants to have printed out
along with the data input listing. All alphabetic labels (UX, FY, EX,
END, etc.) must be left justified in their four space fields . Card
sets requiring sentinel caras for termination are identified in the
37
tables. A card having only a 1 in columns 5 and 6 may be used for
any sentinel card. All geometric input angles are in degrees and out
put rotations are in radians. Right hand coordinate systems are used
throughout except where specifically noted .
4.2.1 ANSYS Input Data for "Static Analysis (ANSYS/Rey. 2)
CARD
CI
COLUMN(S)
TITLE CARD
130
VARIABLE
IHEDD
MEANING
ACCOUNTING CARD
116
18
NAME
NONOTE
Title for output. If columns 7779 are
left blank and a comma punched in col
umn 80, the title may be continued on
the following card. No limit.
(Optional) User Identification Name.
 Print notes (new features, modifi
cations, announcements, etc.) at
end of solution.
1  Suppress printout of notes (con
tinued use not recommended).
(Not Available)
2532 IACCNT (System Option) Account Number
3742 IEQRQD (Optional) Maximum number of equations
in wave front (to check for adequate
core storage) .
7530 ICORE (System Option) Core size parameter.
Note  If no values are input, a blank card is still required.
ANALYSIS OPTIONS
14
7
1112
NSTEPS
K20
KTB
16
K15
Number of load steps (one set of L
through Q cards per load step)
(NSTEPS for an input data check run).
 Static analysis
 No element real constant table
defined
1  Define up to 8 element real
constants per table entry
(Card D2).
N  Define up to N (for N greater
than 8) element real constants
per table entry (Card D2).
 No nodal force output.
1  Calculate and print out nodal
forces for each element and tab
ulate reaction forces at specified
displacement constraints.
K2Q=0
38
CARD COLUMN(S)
CI
(cont.)
16
C2
VARIABLE
K15
MEANING
18
K17
 Print out reaction force tabula
tion only
 Boundary conditions (.Cards N, 0,
P, and Q) are linearly inter
polated within a load step. The
full boundary conditions (as input)
are used in the last iteration of
the load step.
 Boundary conditions are step
changed at the first iteration
to full values defined in the
load step.
22
K23
7475
KPROP
N
 No energy printout.
 Calculate and print out elastic
strain energy for each element.
 Use polynomial material property
equations.
 Use linear interpolation in all
material tables, up to N points
per table (24 max.) .
ANALYSIS OPTIONS (CONTINUED)
112 TREF Reference temperature for thermal
expansions.
1324 TUNIF Uniform temperature (used if no other
temperatures are specified).
ELEMENT TYPES  One card for each element type. End card set
with an 1=0 card.
23
I
Element type number
between 1 and 20) .
(arbitrary,
56
J
Stiffness subroutine for this element.
(A will cause this element type to
be ignored).
7
8
9
10
11
12
KEYSUB(IB)
KEYSUB(IA)
KEYSUBU)
KEYSUBC2B)
KEYSUBC2A)
KEYSUB(2)
Parameter KEYSUBU B)
Parameter KEYSUBU A)
Parameter KEYSUBU )
Parameter KEYSUB(2B)
Parameter KEYSUB(2A)
Parameter KEYSUB(2)
for this subroutine
for this subroutine
for this subroutine
for this subroutine
for this subroutine
for this subroutine
1415
18
KC If J0, enter for KC the stiffness sub
routine number of the element type
being ignored.
INOTPR If 1, suppress all stress and force
printout for this element type.
(Return to next D card)
K2Q=0
39
VARIABLE
MEANING
CARD COLUMN(S)
D2 ELEMENT REAL CONSTANT TABLE  Clnclude this card set only if
KTB is greater than Q on Card CI. The D2 cards may be repeated
to form a table. End table with a blank (or 0.0 in the first
field) card)..
Element real constants (as given for
element stiffness subroutine. Input
constants in the same order as given.
, Several cards may be required for
7180 RC(8) each table entry. Additional constants
on cards are not used) .
110,
RCCD
1120,
RC(2)
2130,
RC(3)
E
El
If a +00000 is punched in columns 16 and the rest of the card
is left blank, suppress the element constant table printout.
If 99999, cancel the suppression.
If a +99999 is punched in columns 16 and a real number (D.) is
input for RC(2) , this card represents D blank table entries.
(Return to next D2 card)
ELEMENT DEFINITION CARDS  one card set (El, E2) for each
element  end with an I=l card.
ELEMENT DESCF.IPTION
16 I
712
1318,1924,
2530,3136,
3742,4348
4954
K, L,
M, N,
0, P
MAT
Number assigned to Node I on element
(first node). If 99999, suppress
element printout. If 99999, cancel
the suppression.
Number assigned to Node J on element
(second node, if any) .
Other node numbers, if required.
Material number of this
blank) .
element (1 if
5560
6166
ITYPE
ITABLE
Element type number for this element
(1 if blank). (Refers to element
types defined on D cards).
 Element real constants, if any, are
included on the next card (Card E2)
K.  Element real constants are included
at entry number K of the D2 card
set.
K2Q=0
40
CARD COLUMN (S) VARIABLE MEANING
El
(cont.)
(The following three parameters are required only for
■ or second level element generation).
6772 IiNUM If positive (first level generation),
INUM is the total number of element
sets generated (including the spe
cified set). The elements input on
this and the next NEL1 El. cards form
the specified set.
If negative (second level generation),
INUM is the total number of element
groups generated (incl uding the NEL
elements in the defined group). The
defined group may include separately
specified and/or first level generated
elements. Columns 166 should be left
blank.
7375 NINC Number by which to increment each
element node number to generate suc
cessive element sets or groups.
(Assumed 1 if left blank).
7678 NEL Number of elements in a specified set
or a defined group to be repeated
(assumed 1 if blank) .
Element limit per set = 960/N (where
N=8 or KTB, if KTB (Card CI) is
greater than 8). No element limit
per group.
798Q KNEXT If positive, the tape unit for add
itional element input data (defaults
to the current input file).
If 1, all of the following elements
have INUM added to each node number.
E2 ELEMENT REAL CONSTANTS  (Include this card set only if the
element has required real constants and if I i ABLE (on the
preceding El card) is zero or blank).
112, RC(1) Element real constants i^as given for
1324, RC(2) element stiffness subroutine. Input
2536, RC(3) constants in the same order as given.
3748, RC(4) Several cards may be required for each
4960, RC(5) table entry. Additional constants on
6172 RC(6) cards are not used).
(Return to next El card)
K20=0
41
CARD COLUMN(S) VARIABLE MEANING
F NODE POINT LOCATIONS  One card for each node specified 
and with an I1 card.
* 16 I If positive, I is the node number
being defined (not a ]] numbers need
to be used) .
If zero (or blank), this card is used
to define a local coordinate system.
If negative, this card is used to
define second level nodal point gen
eration. I is the node number in
crement between successive nodal
point groups.
If 99999, suppress nodal point print
out. If 99999, cancel the suppression.
73 KCS **"* If I is not zero ****
 Nodes input (or generated in global
cartesian coordinates.
1  Nodes input (or generated) in globa"
cylindrical coordinates.
2  Nodes input (or generated) in global
spherical coordinates.
N  Nodes input (or generated) in local
coordinate system N (N greater than
2).
***** If I is zero *"**
 A local cartesian coordinate system
is being defined.
1  A local cylindrical coordinate system
is being defined.
2  A local spherical coordinate system
is being defined.
910 KFILL If I is positive ****
 No first level nodal point genera
tion.
N  Fill in nodes between the previously
specified node and this one, incre
menting node numbers by N and
linearly interpolating the coordinates
(First level nodal point generation).
(N must be positive) .
K20=0
42
CARD
F
(cont.
COLUMN(S)
910
VARIABLE
KFILL
(cont. )
MEANING
*** If I ts zsro ***
N  The local coordinate system being
defined is identified as coordinate
system number N (N greater than Z) .
*■*■*
N 
If I is negative
X'M jfc
1112
!<NEXT
The number of nodal points in the
group to be repeated (defined on
the following F cards). (Second
level nodal point generation).
*** If I is positive ***
N  The tape unit number for additional
nodal point input data (defaults to
the current input file).
*** If I is zero, KNEXT is not used ***
*■*■*
N 
***
If I is negative ***
The total number of nodal point
groups generated (including the
defined group). (Second level
nodal point generation).
Special Combinations *"*"*
If KNEXT=1, all of the following node
numbers have I (positive or negative)
added to them. All other parameters
on the card should be left blank.
For defining nodal points use the appropriate node description
column below. The THXY, .., THRP inputs are for nodal coordinate
rotation. All angles are input in degrees. Use 30 input if a
30 element is included in the D card set.
For local coordinate system definition use Column 3 for origin
translation and coordinate system rotation.
For second level generation, inputs are incremental values.
Increments and nodal points must be specified in the same
coordinate system (KCS).
20imensional
Rectangular Polar
1324
2536
3748
4960
6172
7380
X
Y
THXY
R
THETA
THRT
(Return to next
K20=0
Cartesian
X
Y
Z
THXY
THYZ
THXZ
F card)
30imensional
Cylindrical
R
THETA
Z
THRT
THTZ
THRZ
Spherical
R
THETA
PHI
THRT
THTP
THRP
CARD CQLUMN(S) VARIABLE MEANING
H MATERIAL PROPERTY DEFINITIONS  the H card set CHI , H2) may
be repeated. End with a LABEL=END card.
HI MATERIAL PROPERTY EQUATIONS
14 LABEL LABEL identifying the property
EX EY EZ ALPX ALPY ALPZ NUXY NUYZ
NUXZ DENS MU GXY GYZ GXZ COPR NOPR
END (Note  All labels are left justifies)
(Only properties required by element
material descriptions need be input.
In addition, for isotropic materials,
only the X (or XY) property label need
be input) .
58 MAT Material number (assumed 1, if left
blank).
12 KEY  Polynomial coefficients are input
on this card.
1  A curve must be fit to the set of
temperature vs. property data
points listed on the following H2
cards .
2  Fit curve as described for KEY=1
and print out the fitting equation
coefficients.
3  Use linear interpolation in all
material property tables (input
table on H2 cards). (Note, if KEY=3
for any material, it must be 3 for
all materials).
1324 CO Constant term in the property polynomial
equation.
Coefficient of linear term in equation.
Coefficient of quadratic term.
Coefficient of cubic term.
Coefficient of quartic term.
H2 MATERIAL PROPERTY TABLE  (Included only if KEY is greater than
zero on previous HI card)
First card 
112 POINTS Number of temperature ys. property
points in table. If KEY=1 or 2, at
least 6 property points are required.
If KEY=3, the number of points must
not exceed the KPROP value input on
Card CI.
K20=0
44
2536
CI
3748
C2
4960
C3
6172
C4
CARD COLUMN(S) VARIABLE MEANING
H2
(cont. )
"I 3 " 24 TSTART Temperature corresponding to first
property value input [required only
if DELTAT is greater than zero).
2536 DELTAT Constant value by which, temperatures
are incremented. Temperatures corre
spond to property values input on the
next card(s) .
Following cards  If DELTAT=0.0 (or blank), three temperature
property pairs may be input per card. Tem
peratures must be input in ascending order.
If DELTAT is greater than zero, six properties
may be input per card. Properties correspond
to temperatures generated on first H2 card.
(Continue table on as many cards as required, Format (6E12.2))
(Return to next HI card after table is complete).
LQ The following load cards (LQ) are repeated NSTEPS (Card CI)
times unless the repeating sets are terminated with a KDIS= <3 9
card before the last expected (NSTEPS) set.
L LOAD STEP DEFINITION
13 KDIS 1  Define new values for displacement,
force, and pressure boundary condi
tions. Formulate new stiffness
matrix. Zero all nonlinear terms
and previous boundary conditions.
 Use the previous displacement, force
and pressure boundary conditions
(do not include N, 0, or P card
sets). Reformulate stiffness matrix.
Continue nonlinear analysis.
1  Change some of the previously defined
displacement, force, and pressure
boundary conditions (include changed
values and N, 0, and P card set
terminators). Also use unchanged
previous bounc^ry conditions. Re
formulate stiffness matrix. Conti
nue nonlinear analysis.
2  Same as KDIS=1 except use previously
formulated stiTfness matrix (speci
fied displacement constraints (on
N cards) must be reseated (and all
zero) ) .
K20=Q
45
CARD COLUMN(S)
L 13
(cont. )
VARIABLE
MEANING
kdis a
(cont. )
46
KTEMP
99 

1 
2 
3 
N 
Same as KDIS1 , except use previ
ously formulated stiffness matrix
Cspecified displacement constraints
must remain zero) ,
Terminate the load card sets before
the last expected set. An R or S
card must follow.
Set all temperatures to TUNIF
(Card C2).
Read in element temperatures on the
Q cards for all elements.
Read in nodal point temperatures on
the Q cards.
Use temperatures from previous load
step.
Use the temperatures calculated in
the Nth cumulative iteration
(file TAPE4) of a previous ANSYS
heat transfer solution.
79
NITTER
1012
NPRINT
M
The number of substep (or iterative)
calculations to be done this load step
(defaults to 1). Note, boundary con
ditions are linearly interpolated if
,K17=0. If NITTER is negative, use
covergence options (step boundary con
dition change imposed).
Frequency of printout of stress, force,
and displacement results  only every
NPRINT iteration is printed out, begin
ning with iteration NPRINT. If zero
or blank, suppress all printout for
this load step . If negative, suppress
boundary condition input printout only,
For a negative value of NITTER, if
NPRINT NITTER , print the converged
(or last) iteration. If NPRINT >
NITTER , suppress all solution print
out.
ADDITIONAL LOAD, PLOT, AND PRINT DEFINITION CARD
The following four parameters may be used if more than three
space fields are needed for the corresponding parameters on
the L card.
16
712
KDIS If nonzero, use instead of the value
on Card L.
KTEMP If nonzero, use instead of the value
on Card L.
K20=0
46
CARD COLUMN(S) VARIABLE MEANING
M
(cont.)
1318 NITTER If nonzero, use instead of the value
on Card L.
1924 NPRINT If nonzero, use instead of the value •
on Card L.
N DISPLACEMENT DEFINITION CARDS  The N cards may be repeated.
End with a LABEL=END card.
16 I Node number at which displacement is
specified.
If 99999, suppress displacement printout.
If 99999, cancel the suppression.
If 2, add 12 to all the following nodes,
7 IKEY If j delete this displacement specifi
cati on .
811 LABEL Direction of displacement. (In nodal
coordinate system)
UX UY UZ ROTX ROTY ROTZ PRES END
1324 DISP Value of displacement at this time
(Radians for totations).
3742 12 If 12 is greater than I (for I positive),
4348 15 all nodes from I through 12 in stpes
of 15 have this specified displacement
(.15 is assumed to be 1 , if left blank)
5154, LABELS (5) Additional direction labels for which
5760,6366, this displacement value applies at
6972,7578 this node.
(Return to next N card)
Q FORCE DEFINITION CARDS  The cards may be repeated. End with
a LABEL=END card.
16 I Node at which force acts
If 99999, suppress force printout
If 99999, cancel the suppression
If 2, add 12 to all the following nodes.
811 LABEL Direction of force. (.In r\oda] coordinate
system) FX FY FZ MX MY MZ
FLOW END
K20=0
47
CARD CQLUMN(S) VARIABLE MEANING
(cont. )
1324 FORCE Value of the force at this time.
3742 12 If 12 is greater than I (for I positive),
all nodes from I thru 12 in steps of
15 have this specified force (15 assumed
to be 1 if left blank).
(Return to next Q card)
P PRESSURE DEFINITION CARDS  The P cards may be repeated. End
with a blank (or 1=0) card.
Pressures act in the element coordinate system. See Table 4.J.1
for pressures available for element type J.
16 I Element upon which pressure acts
If 99999, suppress pressure printout.
If 99999, cancel the suppression.
If 2, add 12 to all the following
elements.
712 IFACE Face of element on which pressure acts.
(If a superelement, IFACE is the
load vector number) .
1324 PRESS Value of the pressure at this time.
(If a superelement, PRESS is the
scale factor for load vector IFACE).
3742 12 If 12 is greater than I, all elements
from I through 12 in stpes of 15 have
this pressure on this face (15 is
assumed 1 if left blank).
(Return to next P card)
q TEMPERATURE DEFINITION CARDS  (Include this card set only if
KTEMP1 or 2 on Card L).
Element temperature format (used if KTEMP is 1). One specifica
tion is required for each element, in the same order that the
elements are specified. If KTEMP=2, use the node temperature
format.
18 Tl First temperature for this element.
K2Q=0
48
CARD CQLUMN(S) VARIABLE MEANING
Q ■ 916,... T2,.,. Second temperature, etc.
(cont.) .;, 5764 ...,T8 (Note  Fluences are also Input where
applicable) ,
6572 INUM If or 1, one element has this set of.
temperatures.
If N, the neat N elements (.counting
this element) have these temperatures.
7374 KNEXT If positive, subsequent temperature
input is to be from tape KNEXT (defaults
to the current input file).
76 KTCONT  All temperatures and fluences to
be specified are contained on this
card.
1  Additional temperatures and fluences
continued on next card.
Note  If KTC0NT=1 , T9 through T16 should be input on the next
(second) card. The continuation card format is the same as the
first card except that INUM and KNEXT are not used. Values not
input are assumed to be zero.
If a +99999 is punched in columns 16, suppress the element
temperature printout. If 99999, cancel the suppression.
(If all element temperatures have not
been specified, return to next Q card).
Nodal point temperature format (used if KTEMP is 2). Nodal
temperature specification cards may be repeated. Nodal
temperatures not specified are set equal to TUNIF (Card C2).
End nodal temperature set with an I=l card.
16 I Node number at which temperature is
specified (if 1, end of nodal tem
perature input) .
If 99999, suppress nodal temperature
printout.
If 99999, cancel the suppression.
If 2, add 12 to all the following nodes.
Specified nodal temperature.
Specified nodal fluence.
If 12 is greater than I (for I positive),
all nodes from I through 12, in steps of
15, have this temperature (15 is assumed
to be 1 if left blank).
K2Q=0
49
1324
TEMP
2536
FLUEjNCE
3742
4348
12
15
CARD CQLUMN(S) VARIABLE MEANING
Q
( cont ) (Return to next Q card)
(Return to neat L card tf another load step is to be defined).
S END OF DATA DECK CARD
16 FINISH The word FINISH is punched in Columns 16
of the last card of a problem data deck.
Another problem data deck (oeginning
with Card A) may follow.
K20=Q
50
Oftentimes for real life problems, the engineer will have to use
the 3rd Revision of ANSYS (Extended Core Version). To go from the
2nd Revision to the 3rd one, set NSTEPS  Q [solution problem} or
NSTEPS 3 1 (model check problem) on card CI and finish with LQ card
sets with a KDISEND card.
4.2.2 ANSYS Input Data, for w«t Transfer Analysis (ANSYS/ Rev. 2)
CARD COLUMN (S) VARIABLE MEANING
A
B
TITLE CARD  See section 4.2.1 for data input instructions.
ACCOUNTING CARD  See section 4.2.1 for data input instructions.
CI ANALYSIS OPTIONS
14 NSTEPS
67
K20
112
KTB
1
N
16
K15
1
2
18
K17
32
KAY(2)
Number of load steps (one set of L
through Q cards per load step).
(NSTEPS for an input data check run).
1  Heat Transfer analysis.
No element real constant table
defined.
Define up to 8 element real con
stants per table entry (Card 02).
Define up to N (for N greater than
8) element real constants per
table entry (Card D2).
No nodal heat flow rate printout.
Calculate and print out nodal heat
flow rate for each element and
tabulate heat flow rates at speci
fied temperature constraints.
Print out heat flow rate tabulation
only.
Boundary conditions (Cards N, 0, P,
and Q) are linearly interpolated
within a load step. The full bound
ary conditions (as input) are used
in the last iteration of the load
step.
1  Boundary conditions are step changed
at the first iteration to the full
values defined in the load step.
 First order integration for trans
ient solutions.
<20=l
51
CARD
CI
(cont. )
COLUMN(S)
32
7475
VARIABLE
KAY(2)
(cont. )
KPROP
MEANING
77
K18
1  Second order integration for trans
ient solutions (recommended)
(required for convergence or
optimization procedures).
 Use polynomial material property
equations.
N  Use linear interpolation in all
material tables, up to N point
per table (24 max. ) .
 Nodal coordinate directions rotated
for nodes input in global cylin
drical and global spherical coordi
nates (nodal xaxis is along input
radius unless otherwise specified
on F card.
C2
ANALYSIS OPTIONS (CONTINUED)
1324
4954
NUMEL
5560
MAXNP
6164
KRSTRT
6568
TOFFST
6975
TUNIF Used only if KDIS=1 . If so, all nodal
temperatures , the temperature boundary
conditions (Card N) and the bulk tem
peratures (Card P) at the beginning
of the load step are set to TUNIF.
Also temperature dependent material
properties are evaluated at TUNIF for
the first iteration.
Number of elements (required only for
restart).
iMaximum node number (required only for
restart).
The last load step already done,
(restart key) .
Degrees between absolute and of
temperature system used (required for
radiation) .
TRSTRT Time at end of run to be continued
(required only for restart}.
ELEMENT TYPES  See Section 4.2.1 for data input instructions
Note, the INOTPR parameter is used to suppress all heat
flow printout for this element type.
K2Q=1
52
CARD COLUMN(S) VARIABLE MEANING
D2 ELEMENT REAL CONSTANT TABLE  (Include this card set only if KTB
is greater than on Card CI .
See section 4.2.1 for data input
instructions) .
E ELEMENT DEFINITION CARDS  See Section 4.2.1 for data input
instructions.
F NODE POINT LOCATIONS  See Section 4.2.1" for data input instructions
H .MATERIAL PROPERTY DEFINITIONS  See Section 4.2.1 for data input
instructions.
Note, the list of structural property labels (Cols. 14) should
be replaced with the following thermal property identification
list.
KXX KYY KZZ DENS C HF OHMS VISC EMIS NOPR GOPR END
LQ The following load cards (LQ) are repeated NSTEPS (Card CI)
times unless the repeating sets are terminated with a KDIS=99
card before the last expected (NSTEPS) set.
L LOAD STEP DEFINITION
13 KDIS 1  Define new values for temperature,
heat flow, and convection boundary
conditions. Formulate new conduc
tivity and specific heat matrices.
Zero all transient terms and pre
vious boundary conditions.
 Use the previous temperature, heat
flow, and convection boundary con
ditions (do not include N, 0, or
P card sets). Re formulate matrices
Continue transient analysis.
1  Change some of the previously de
fined temperature, heat flow, and
convection boundary conditions
(include changed value's and N, 0,
and P card set terminators). Also
use unchanged previous boundary
conditions. Reformulate matrices.
Continue transient analysis.
K20=l
53
CARD COLUMN(S)
L 13
(cont.)
46
VARIABLE
KDIS
(cont. )
KTEMP
MEANING
99 

1 
3 
Terminate the load card
the last expected set.
card must follow.
sets before
An R or S
Set all internal heat generation
rates to 0.0.
Read in element internal heat gener
ation rates on the Q cards for all
elements.
Use heat generation rates from pre
vious load step.
79
NITTER
1012
NPRINT
M
The number of substep (or iterative) ■
calculations to be done this load step
(defaults to 1 ) . Note, if K17=0,
boundary conditions are linearly inter
polated. If NITTER is negative, use
steadystate convergence (step boundary
condition change required) or transient
optimization procedure.
Frequency of printout of heat flows and
temperature results  only every NPRINT
iteration is printed out, beginning
with iteration NPRINT. If zero or
blank, suppress all printout for this
load step ! If negative, suppress boun
dary condition input printout only.
For a negative value of NITTER, if
NPRINT= NITTER , print the converged
(or last) iteration. If NPRINT >
NITTER , suppress all solution printout.
Time characterizing the end of this load
step (If TIME is 0.0, blank, or less
than the time of the previous load step,
a steadystate solution is done).
ADDITIONAL LOAD, PLOT, AND PRINT DEFINITION CARD
The following four parameters may be used if more than three
space fields are needed for the corresponding parameters on
the L card.
If nonzero, use instead of ' the value on
Card L.
If nonzero, use instead of the value on
Card L.
If nonzero, use instead of the value on
Card L.
If nonzero, use instead of the value on
Card L.
K2Q=1
1324
TIME
16
KDIS
712
KTEMP
1318
NITTER
1924
NPRINT
54
CARD COLUMN(S)
VARIABLE
MEANING
N
TEMPERATURE DEFINITION CARDS  The N cards may be repeated. End
with a LABELEND card.
15
I
7
311
1324
3742
4348
IKEY
LABEL
TEMPER
12
15
Node number at which temperature is
specified.
If 99999, suppress temperature printout.
If 99999, cancel the suppression.
If 2, add 12 to all the following nodes.
If , delete this temperature specifica
ti on .
Input one of the following words
(left justified) .
TEMP PRES VOLT END
Value of temperature (etc.) at this time.
If 12 is greater than I (for I positive),
all nodes from I through 12 in steps of
15 have this specified temperature (15
is assumed to be 1 , if left blank).
(Return to next N card)
CONVECTION DEFINITION CARDS  The P cards may be repeated. End
with a blank (or 1=0) card.
16
I
712
1324
IFACE
HCOEF
2536
TBULK
Element upon which convection acts.
If 99999, suppress convection printout.
If 99999, cancel the suppression.
If 2, add 12 to all the following
elements.
Face^f element on which convection acts.
If a. superelement, IFACE is the load
vector number.
Value of the film coefficient at this
time. Note, if KDIS1 , the film
coefficient at the beginning of this
load step is also set to this value.
If N., use HF vs. TFILM equation input
for material N on the H cards.
If a superelement, HCOEF is the scale
factor for load vector IFACE.
Bulk temperature of adjacent fluid at
this time.
K2Q=1
55
CARD COLUMN(S) VARIABLE MEANING
P TBULK
(cont. ) (cont.)
3742 12 If 12 is greater than I (for I positive),
"4343 15 all elements from I through 12 in steps
of 15 have this convection on this face
(15 is assumed to be 1 if left blank).
(Return to next P card)
Q HEAT GENERATION RATE DEFINITION CARDS  (Include this card set
only if KTEMP1 on Card L. One speci'
fi cation is required for each element,
in the same order that the elements
are specified) .
13 HTGEN Internal heat generation rate for
or CI this element.
916, C2,— Constants defining polynomial equation
— ,5764 — ,C8 for variable heat generation rate
(applicable to STIF71 elements).
6572 INUM If or 1 , one element has this rate.
If N, the next N elements (counting
this element) have this rate.
7374 i KNEXT If positive, subsequent heat generation
rate input is to be from tape KNEXT
(defaults to. the current input file).
If a +99999 is punched in Columns 16, suppress the internal
heat generation rate printout. If 99999, cancel the sup
pression.
(If all element heat generation rates have not been specified
return to the next Q card).
(Return to next L card if another
load step is to be defined)
S END OF DATA. DECK CARD
16 FINISH The word FINISH is punched in Columns
16 of the last card of a problem data
deck. Another problem data deck (begin
ning with Card A) may follow.
•K20=l
56
4.2.3 ANSY5 Input Data for Thermal Stress Analysis
The thermal stress is equivalent to the static analysis except
as follows:
1. Save file TAPE 4 from heat transfer analysis.
2. Assign file TAPE 4 to thermal stress analysis.
3. Set KTEMP=N (read temperatures fo the Nth iteration of
previous heat transfer solution from file TAPE 4).
Table 4.1 Element Reordering Instructions
FIELD COLUMNS VARIABLE MEANING
CARD Fl **** ELEMENT REORDERING INSTUCTIONS— Use as many cards as necessary
to define a starting wave set. Use additional cards to define
additional starting wave sets. End Fl card set with and Nl=
END card.
First node, second node, third
node, etc., on starting wave.
Continue on additional cards
if necessary (Format 1216).
12 6772 N12 Blank fields are ignored.
End starting wave list with
a 1 node number.
1
16
Nl
2
712
N2
3
1318
N3
(Return to next Fl card)
57
a
SJ
<S3
S
a
C5
s_
oj
s.
o
<u
CM
cu
23
3j
' 3
3 S
_j
m
:q
la
COI
H
i>— !
:cni
Si!
a\ ;
£li 1
.■I j
>■■ 
l ! r 1
;
i»i
' i
r
1
1
!«i
5.
J)
1
! 1
i*i
3?
S
1

h
5)
1 1
. \i
V
=1 
:•
1
: ! I
, L,
^
1
i i !
l ill
1 l;j
SI
1
i
St
=1
SI
;). 
1
i
1 1
jsi
21 1
i 1
i r
i : ,
Ui
SI
:
1st
31
1 :
:
ill HI
1
i i
! lal
31 >
i
I SI
31
■
II
u :
_1 ;1
St
^ 1
i
51
i r.. 1 i
>SI
i
=1 i
Ui

i
N
il
i
l
i
i
1
V i
r
I
;
jsi
sj
r <
i
1
=1
'
! i
I
i"
=r^ " "
i l i
1 1
■ s
2)
I !
!
1
\a'i
5 ;
:
1=1
SI
1
1
1 :
i
i Ui
SI

1
!
:
I = i
=!
1 i
;
"! ' l=i
=1
1 i
i ; i
31
i
SI
SI !
: i
IS!
31 1 1
i j«j
SI
i
j  j
SI l
■s
SI
1
!sl
si
I sj
si
1
'!
S
i
! 1
Z3°i
S
1
i
'•■
i
1
: i
• 'i
S !
1
1 :
1 ;
i il
*l i
1
i
1
I 1
I s !
1 i
<~\
M
!
i
Ul
=r~
1
i
1 i
! i
r\
SI 1 !
! !
: l
i i ;
: i
1 I s !
=i
i
'
'=1
=ii'.
! i
"' ' .31
=i
i
1=1
»! i i ■
!
1
! i i
l«
SI I
1
!
i ; i
,= i
81
i
; : i
i
i
!s
sj
i
i i
i
1
'SI
= 1
i i
; 1
i i
~i
= 1 1 ' ■
1 :
! i 1
j ! ill
i
i s !
S) i !
i 1
l i 1
i
ii
=1  . : •
i i
!
i
I s !
[ l
! i
i i
!ai !
=j
r
I
■z\=.
*j f ;
ii !
1
i ;
; *i
St 1 '
f ! 1
! I
: i
S?
si I
y
' i ' l
j_ i
i
i H
1 j ;
!
l=j
=i
i
l s U
!
; i
f— '
\U
=t ■!
1
j 
i . r is
i
! i
=t
i
,1 I ,
1 :
I
!
—
H§
.1 1
! i
!
' i
■ "'*
 i 1. i .
I :
: j i
1
'I.:
r»c5ticj!cvji^c3v —
' *\
, pjaSto^ssij
I
— 
iiJ
: i
■!
lll
x *
1
CJ
3 
1 , i
"3>"
. ., .
! — :m(
LUl
■ '.
58
Y
Sk
A
A
A
A
A
/\ = Element Number
NX=3
NY6
NZ=4
ny)nz)nx
NOTE THAT ThFoRDERING OF THE NOOES IS THE SAME AS IN FIGURE 3.1
WAVE FRONT=(NX)(NZ) (DEGREES OF FREEDOM PER NOOE)
Figure 4.1 Example of Element Reordering to Minimize
the Wave Front
59
CHAPTER 5
ELEMENT LIBRARY OF ANSYS
5.1 ELEMENT SELECTION
Table 5.1 is a summary of the available elements in ANSYS program.
The above table lists the element identification number, the name, the
number of dimensions, the number of degrees of freedom per node, the
number of nodes, and some features.
ANSYS models are either twodimensional or threedimensional,
depending upon the element types used. Twodimensional models must be
defined in the xy plane and the nodes must be input using the two
dimensional format on the F cards. Threedimensional models must be
defined in the xyz plane and the nodes must be input using the three
dimensional formate on the F cards. The element input is included on
the ANSYS program data input cards as shown in Table 5.2.
The degrees of freedom associated with the model should be suffi
cient to characterize the actual response. Including unnecessary degrees
of freedom or selecting elements with unnecessary features increases
the solution core size and running time.
The units of the element input and output parameters are described
in Table 5.3 in terms of force (F), length (L), time (t), temperature
(T), and heat (Q). Mass units can also be expressed as Ft 2 /L.
5.2 ELEMENT LIBRARY FOR STATIC ANALYSIS
The threedimensional isoparametric element (STIF45) and the
threedimensional interface element (STIF52) are recommended to use
in a static analysis.
5.2.1 Threedimensional Isoparametric Solid Element
The threedimensional isoparametric solid element is a higher
order version of the threedimensional elastic solid element (STIF5).
The higherorder element gives a considerable improvement of accuracy
over the constant strain element. The advantage of isoparametric
elements over constant strain elements is that, for a given accuracy,
the number of degrees of freedom necessary to describe the structure
may be reduced. Accordingly, not only the data preparation time, but
also the computer wave front solution time is reduced.
The element has plasticity, but no creep or swelling capabilities.
If all capabilities are needed, STIF49 should be used. The isoparametric
solid element is defined by eight nodal points having three degrees of
freedom at each node: translations in the nodal x, y , and z direction.
An option is available to print out the stresses and strains on
particular element surfaces when the surfaces are fr^e surfaces of the
structure. Other options are available to print stresses at the inte
gration points or at the nodes. A summary of the isoparametric solid
60
element parameters is given in Table 5.4.
Input Data . The geometry, nodal point locations, face numbers,
loading, and the coordinate system for this family of elements are
shown in Fig. 5.1. The element is defined by eight nodal points and
the material properties. The nodal points should be numbered in the
order shown in Fig. 5.1. The number of nodes input on Card El defines
the type of solid element used. The material" may. be orthotropic, with
ten elastic constants required for its specification. The three addi
tional shear modulus terms are optional and may be included for a more
complete description of the material. If not included, the values are
computed from the other input properties. There are no real constants
required for this element.
The element loading can be either temperature gradients (specified
by nodal temperatures) or pressures (on one or more faces), or a
combination of both.
The data input for the isoparametric solid element is as follows:
1) only the eight node element with six pressure surfaces is available;
2) plasticity capability is included; 3) printout is available on a
second surface for elastic solutions, as the numerical integration
points, and at the nodal points; 4) the incompatible displacement modes
may be suppressed with KEYSUB(IB), and 5) the number of number integra
tion points may be selected for elastic solutions with KEYSUB(IA).
Output Data . The solution printout associated with the isopara
metric solid element is summarized in Table 5.5. Figure 5.2 shows a
schematic STIF45 element output.
Theory . The element formulation includes incompatible displacement
modes. Either a 3x3x3 or a 2x2x2 lattice of integration points is
available for use with the numerical (Gaussian) integration procedure.
Assumptions and Restrictions . Zero volume elements are not allowed.
Elements may be numbered either as shown in Fig. 5.1 or may have the
planes IJKL and MNOP interchanged. Also, the element may not be twisted
such that the element has two separate volumes. This occurs most fre
quently when the elements are not numbered properly. The dihedral angle
between adjacent element faces should be less than 180°.
All elements must have eight nodes. A "triangular" shaped element
may be formed by defining duplicate K and L and duplicate and P node
numbers. The extra mode shapes are automatically deleted for
"triangular" shaped elements so that a "constant strain" element re
sults.
The first two lines of the element solution printout are valid for
both isotropic and orthotropic materials. The principal strains (line
3) are not valid for orthotropic materials. The principal stresses and
the maximum shear stresses, however, are valid for orthotropic materials.
61
Surface stress outputs are valid only for isotropic elastic
materials for which this face is a fr^e surface of the structure.
Surface stresses should not be requested on the zero area face of
"triangular" shaped elements.
The 2x2x2 lattice of integration points is automatically used
with plasticity solutions (K13 > on Card CI).
5.2.2 Threedimensional Interface Element
The threedimensional interface element represents two parallel
surfaces in space which may maintain or break physical contact and
may slide relative to each other. The element is capable of supporting
only compression in the direction normal to the surfaces and shear
(Coulomb friction) in the tangential directions. The element has
three degrees of freedom at each node: translations in the nodal x,
y, and z directions.
The element may be initially preloaded in the normal direction
or it may be given a gap specification. A specified stiffness acts in
the normal and tangential directions when the gap is closed and not
sliding. Because of the nonlinearity of the element an iterative
solution procedure is required. A summary of the threedimensional
interface element parameters is given in Table 5.6.
Input Data . The geometry, nodal point locations, and the coordi
nate system for the interface element are shown in Fig. 5.3. The
element is defined by two nodal points, an interface stiffness, an
initial gap (or interference, and an initial element status. The
orientation of the interface plane (unlike STIF12) is defined by the
nodal point locations. The plane is assumed to be perpendicular to
the 10 line. The element coordinate system has its origin at node
I and the xaxis is directed toward node J. The interface plane is
parallel to the element y, z plane.
The stiffness, k, may be computed from EA/L  where the parameters
are determined from the adjacent element. The effective length, L e «,
is arbitrary, but may be on the order of 1/10 of the adjacent element
length. The stiffness may also be computed from the maximum expected
force divided by the maximum allowable surface displacement. In most
cases k is several orders of magnitude greater than the other stiff
nesses in series with it so that its exact value is not critical. The
initial gap (GAP) may be positive or negative. 'If negative, an ini
tial interference of this amount exists. The initial element status
(START) is used to define the "previous" condition of the interface
to be used at the start of the first iteration. This input overrides
the condition implied by the gap specification and is useful in anti
cipating the final interface configuration and thereby reducing the
number of iterations required for convergence. This parameter is also
useful for inputting the element status in a run which is to be con
tinued, as determined from a previous ANSYS run.
S2
The only material property required is the interface coefficient
of friction, u. A zero value should be used for friction less surfaces.
Temperatures (used if u is temperature dependent) may be specified at
the element nodes. For some problems, a loss of contact or a sliding
at the interface isolates a portion of the structural model not having
sufficient displacement constraints. The KEYSUB(l) option, therefore,
may be used to maintain a small force across and along the interface,
maintaining stability while causing only a negligible inaccuracy in the
analysis. The KEYSUB(2) option may be used whenever friction may cause
some gap elements to oscillate slightly between a sliding and a stick
ing status.
Output Data . The solution printout associated with the three
dimensional interface element is summarized in Table 5.7. The value
USEP is the normal displacement (in the element xdi recti on) betw een
the interface surfaces at the end of this iteration, that is, USEP =
(u ),  (u ) + GAP. This value is used in determining the normal
force. Note, the normal force will not be an equilibrium value unless
this iteration represents a converged solution.
The value USLIDE is the accumulated amount of surface sliding at
the end of this iteration. Sliding may occur in both the element y and
z coordinate directions. Note, sliding occurs in the iteration after
the limiting tangential force is exceeded. KTYPE describes the status
of the element at the end of this iteration for use in the next itera
tion. The surface may be in rigid contact (KTYPE=1), sliding contact
(KTYPE=2), or frze (KTYPE=3). If, for example, KTYPE* 3 at the end of
an iteration, an element stiffness of zero is used for the next itera
tion. The KTYPE values may be input *or START if a new run is to
continue from this iteration.
If no other effects are present ':nd KEYSUB(2)=0, convergence
occurs whenever the gap status remains unchanged. For a friction! ess
surface, the converged gap status is either KTYPE=2 or 3. Whenever
KEYSUB(2) > 0, an element having sliding force oscillations within a
defined tolerance range on u F , resulting in an oscillating gap
status (KTYPE=1 , 2, etc.), is accepted as converged. This tolerance
range is usually within the uncertainty range of u.
Theory . The displacement functions for the interface element
can be separated into the normal and tangential directions since they
are basically independent. In the normal (element x) direction, when
the normal force (F ) is negative, the interface remains in contact
n
and responds as a linear spring. As the normal force becomes positive,
contact is broken and no force is transmitted (unless !<EYSUB(1 )=1 ,
then a small force is supplied to prevent a portion of the structure
from being isolated).
In the tangential directions, for F < and the absolute value
of the tangential force (F ) less than or equal to (u F n ), the inter
face does not slide and responds as a "linear spring in the tangential
63
direction. However, for F„ < Q and F„ > u F„ , sliding occurs. Note
n s r n
that F„ is a variable and if contact fs broken, the tanaential function
n
degenerates to a zero slope straight line through the origin (or of
slope K/1Q\ if KEYSUB(IH) indicating that no Cor little) tangential
force is required to produce sliding. Figure 5,4 shows the displace
ment functions for this element.
Assumptions and Restrictions . The gap size may be specified
independently of the nodal point locations. Nodes I and J, however,
may not be coincident since the nodal locations define the interface
plane orientation. The element is defined such that a positive normal
displacement (in the element coordinate system) of node J relative to
node I tends to open the gap. Recall that the element coordinate
system is defined by the I and J node locations. The nodes defining
the element may have arbitrarily rotated nodal coordinate systems
since a displacement transformation into the element coordinate system
is included.
The friction coefficient may be input as a function of temperature
and is evaluated at the average of the two node temperatures. For this
nonlinear element an iterative solution procedure is required with the
stiffness matrix re formulation each iteration. Note, the effect of
the element status changed in this iteration does not appear until the
next iteration. Nonconverged solutions are not in equilibrium. If
GAP=0.Q (or blank), the element stiffness is included in the first
iteration, unless START=3.0.
The element operates only in the Static (K2O0) and the Nonlinear
Transient Dynamic (K2Q=4) analyses. If used in other analysis types,
the element maintains its initial status throughout the analysis.
Note, a gap condition capability is also included in the Reduced Linear
Transient Dynamic (K20=5) analysis.
The element coordinate system orientation angles a and 8 (shown
in Fig. 5.3) are computed by the program from the nodal point locations,
a ranges from 0° to 360° and S from 90° to +90°. Elements lying
along the +Z axis are assigned values of a=0°, S= + 90°, respectively.
The element coordinate system for a=0°, 8=90° is shown in Fig. 5.3.
Elements lying off the Zaxis have their coordinate system oriented as
shown for the general a, 2 position. Note, for a=90°, 3^90°, the
element coordinate system flips 90° at the Zaxis.
5.3 ELEMENT LIBRARY FOR HEAT TRANSFER
For a heat transfer analysis, it is recommended to use the iso
parametric quadrilateral temperature element (STIF55) and the two
dimensional conducting bar (STIF32).
5.3.1 Isoparametric Quadrilateral Temperature Element
The isoparametric quadrilateral temperature element can be used
as a biaxial plane element or as an axisymmetric ring element with a
twodimensional thermal conduction capability. The element has four
64
nodal points with a single degree of freedom, temperature, at each node.
The isoparametric temperature element. is a higherorder version of the
twodimensional linear temperature element (STIF35). The advantage of
isoparametric temperature elements over linear temperature elements is
that, for a given accuracy, the number of degrees of freedom necessary
to describe the structure may be reduced. Accordingly, the data pre
paration time and the computer wave front solution time are also reduced.
The isoparametric temperature element is applicable to a two
dimensional, steadystate or transient, Thermal (K20=l) analysis. If
the model containing the isoparametric temperature element is also to
be analyzed structurally, the element should be replaced by an equiva
lent structural element. The nodal temperatures determined from the
isoparametric temperature element are applied to the corresponding
structural nodal points. A summary of the isoparametric quadrilateral
temperature element parameters is given in Table 5.8.
Input Data . The geometry, nodal point location, face numbers,
loading and the coordinate system for the isoparametric temperature
element are shown in Fig. 5.5 The isoparametric temperature element
must have four nodes.
The thermal conductivities are defined in the global X and Y
directions. The specific heat and the density may be assigned any
values for steadystate solutions. An average internal heat generation
rate may be applied to the element. All of the element lateral surfaces
have convection capability and are numbered as shown in Fig. 5.5.
Output Data . The solution printout associated with the isopara
metric tamperature element is as shown in Table 5.9.
Theory . The theory on which the isoparametric temperature element
is based as described for the STIF35 element, except for the tempera
ture function. The temperature function in this element is not a
linear polynomial, but includes additional incompatible temperature
modes.
A 3x3 lattice of integration points is used for the
numerical (Gaussian) integration procedure.
Assumptions and Restrictions . The isoparametric quadrilateral
temperature element must not have a negative or a zero area. The
element must lie in an XY plane and the Xaxis must be the radial
direction for axi symmetric problems. Also, axi symmetric structures
should be modeled in the +X quadrants.
A triangular elememt may be formed by defining duplicate K and L
node numbers. The extra mode shapes are automatically deleted for tri
angular elements so that a linear temperature element results. Face 3
should not be defined as a convection surface if nodes K and L are
coincident.
If the thermal element is to be replaced by an analogous structural
element with surface stresses requested, the thermal element should be
oriented such that face 1 and/or face 3 is a free surface.
65
5.3.2 Twodimensional Conducting Bar
The twodimensional conducting bar is a uniaxial element with the
ability to conduct heat between its nodal points. The element has a
single degree of freedom, temperature, at each node point. The con
ducting bar is applicable to a twodimensional (plane or axi symmetric)
steadystate or transient Thermal (K20=l ) analysis.
If the model containing the conducting bar element is also to be
analyzed structurally, the bar element should be replaced by an equiva
lent structural element. The node temperatures determined from the
conducting bar element are applied to the corresponding structural
element's nodal points. Structural elements accepting a transverse
temperature gradient are given a uniform temperature in that direction
by averaging the nodal temperatures. A summary of the twodimensional
conducting bar element parameters is given, in Table 5.10.
Input Data . The geometry, nodal point locations, loading, and
coordinate system for the conducting bar element are shown in Fig. 5.6.
The element is defined by two nodal points, a crosssectional area, and
the material properties. Note that for an axi symmetric analysis, the
area must be defined on a "per radian" basis. The specific heat and
the density may be assigned any values for steady state solutions. The
thermal conductivity is in the element longitudinal direction. An
average internal heat generation rate may be applied to the element.
Output Data . The solution printout associated with the conducting
bar element consists of the node temperatures, T(I) and T(J), which are
included in the overall nodal temperature solution printout.
Theory . The temperature distribution for this element is obtained
from the numerical solution of the following equation:
where K s thermal conductivity (Heat/Length*Time*Deg)
p = density (Weight (or Mass)/Volume)
C = specific heat (Heat/Weight (or Mass)*0eg)
q ■ internal heat generation rate (Heat/Volume*Time)
The temperature function is a, linear polynomial of the form:
T(x) = CJ + C 2 x
where the xaxis extends from node I to node J.
Assumptions and Restrictions . Heat is assumed to flow only in the
longitudinal element direction. The element must be in an XY plane
and the global Xaxis must be the radial direction for axi symmetric
problems. The element must not have a zero length, so nodes I and J
must not be coincident.
66
5.4 ELEMENT LIBRARY FOR THERMAL STRESS ANALYSIS
It is recommended to use the twodimensional isoparametric
element (STIF42) and the twodimensional interface element (STIF12)
in a thermal stress analysis.
5.4.1 Twodimensional Isoparametric Element
The twodimensional isoparametric element is a higherorder version
of the twodimensional constant strain element (STIF2). The higher
order element gives a considerable improvement of accuracy over the
constant strain element. The advantage of more complex elements over
constant strain elements is that, for a given accuracy, the number of
degrees of freedom necessary to describe the structure may be reduced.
Accordingly, the data preparation time and the computer wave front
solution time is also reduced. The element has plasticity, but no
creep or swelling capabilities. If all capabilities are needed,
STIF2 should be used.
The isoparametric element is defined by four nodal points having
two degrees of freedom at each node: translations in the nodal x and
y directions. The element may be used as a biaxial plane element or
as an axisymmetric ring element. An option is available to print out
the stresses and strains on particular surfaces of the element when
the surfaces are free surfaces of the structure. .Other options are
available to print stresses at the integration points or at the nodes.
A summary of the twodimensional isoparametric element parameters is
given in Table 5.11 .
Input Data . The geometry, nodal point locations, face numbers,
loading, and the coordinate system for this element are shown in Fig.
5.7. The element input data includes four nodal points, a thickness
(for a plane stress option only) and the orthotropic material proper
ties. The element loading may be input as any combination of node
temperatures, node fluences, and element pressures. The nodal forces
should be input per unit of depth for a plane analysis (except for
KEYSUBO ) s 3) and per radian for an axisymmetric analysis.
The data input for the isoparametric element is as follows:
1) only the fournode element with four pressure surfaces is available;
2) creep and swelling capabilities are not included; 3) printout is
avaiable on a second free surface for elastic solutions, at the numeri
cal integration points and at the nodal points; and 4) the incompatible
displacement modes may be suppressed.
Output Data . The solution printout associated with the two
dimensional isoparametric element is summarized in Table 5.12. Line
KL is analogous to line I J except that it applies to the opposite
surface. Figure 5.8 shows a schematic STIF42 element output.
Theory . The element formulation includes incompatible displace
ment modes. A 3x3 lattice of integration points is used with the
numerical (Gaussian) integration procedure.
67
Assumptions and Restrictions . The area of the element must be
positive. Zero area elements will print out an error message and con
tribute nothing to the total stiffness. Negative area elements print
out a warning message and will not plot correctly. The numbering of
the nodes should be counterclockwise in the coordinate system shown
in Fig. 5.7. The twodimensional isoparametric element must lie in
an XY plane and the global Xaxis must be the radial direction for
axi symmetric problems. An axi symmetric structure should be modeled
in the +X quadrants,
A triangular element may be formed by defining duplicate K and L
node numbers. The extra mode shapes are automatically deleted for
triangular elements so that a constant strain element results. The
surface stress printout is valid only for isotropic, elastic elements
for which this face is a fr^e surface. Surface strains, however, are
valid for both isotropic and orthotopic elements. Surface stress
printout on an X=0 face of axi symmetric elements or on the zero length
side of a triangular element should not be requested.
5.4.2 Twodimensional Interface Element
The twodimensional interface element represents two plane or
axisymmetric surfaces which may maintain or break physical contact and
may slide relative to each other. The element is capable of supporting
only compression in the direction in the normal to the surfaces and
shear (Coulomb friction) in the tangential direction. The element has
two degrees of freedom at each node:, translations in the nodal x and
y directions.
The element may be initially preloaded in the normal direction or
it may be given a gap specification. A uniform stiffness acts in the
normal and tangential directions. Because of the overall nonlinearity
of the element an iterative solution procedure is required. A summary
of the twodimensional interface element parameters is given in Table
5.13.
Input Data . The geometry, nodal point locations, and the coordi
nate system for the interface element are shown in Fig. 5.9. The
element is defined by two nodal points, an angle to define the inter
face plane, a stiffness, an initial displacement interference, and an
initial element status. The stiffness, if left eq ual to zero, defaults
to 10 s . An element coordinate system (xy) is defined on the inter
face plane. The angle 9 is input in degrees and is measured from the
global X axis to the elementx axis. Note, the orientation of the
interface plane is defined by. the angle 9 and not by the nodal point
locations.
The stiffness, k, may be estimated from EA/L  where the para
meters are determined from the adjacent element. The effective length,
Lxra is arbitrary, but may be on the order of 1/10 of the adjacent
element length. The stiffness may also be computed from the maximum
expected force divided by the maximum allowable surface displacement.
In most cases k is several orders of magnitude greater than the other
68
stiffnesses in series with it so that its exact value is not critical.
The stiffness should be "per radian" for an axt symmetric analysis.
The initial displacement interference, 6, defines the displacement
interference (if positive) or the gap size (.if negative). The Initial
element status (START) is used to define the "previous" condition of
the interface to be used at the start of the first iteration. This
input is used to override the condition implied by the interference
specification and is useful in anticipating the final interface confi
guration and reducing the number of iterations required for convergence.
This procedure may also be used to continue a previous analysis .
The on.ly material property required is the interface coefficient of
friction, u. A zero, value should be used for friction less surfaces.
Temperatures may be specified at the element nodes. For some problems,
a loss of contact or a sliding at the interface isolates a portion of
the structural model not having sufficient displacement constraints.
The KEYSUB(l) option may be used to maintain a small force across and
along the interface, maintaining stability while causing a negligible
inaccuracy in the analysis. The K£YSUB(2)=1 option should be used
whenever friction is present and there is the possibility of some gap
elements oscillating slightly between a slidingsticking status.
Output Data . The solution, printout associated with the two
dimensional interface element is summarized in Table 5.14.
The value USEP is the normal displacement between the interface
surfaces at the end of this iteration, that is: USEP = (u ) ,  (u w ) T  <3
y « y i
This value is used in determining the normal force. For an axi symmetric
analysis, the element forces are expressed per radian of circumference.
The value USLIDE is the accumulated amount of surface sliding at the end
of this iteration.
KTYPE describes the status of the element at the end of this itera
tion. It KTYPE=1 , the gap is closed and no sliding occurs. If KTYPE=3,
the gap is open. If at the end of an iteration KTYPE=3, an element
stiffness of zero is used for the next iteration. A value of KTYPE=+2
indicates that node J moves to the right of node I as shown in Fig. 5.9.
KTYPE=2 indicates a negative slide. If no other effects are present
and KEYSUB(2)=0, convergence occurs whenever the element status remains
unchanged. For a frictionless surface (u=0.0), the converged element
status is either KTYPE=+2 or 3. Wherever KEYSUB(2) > 0, an element
having sliding force oscillations within a defined tolerance on
U F , resulting in an oscillating element status (KTYPE=1, 2, etc.),
is accepted as converged. This tolerance range is usually within the
uncertainty range of u.
Theory . The displacement functions for the interface element can
be separated into the normal and tangential directions because they are
basically independent.
In the normal direction, when the normal force (F ) is negative,
the interface remains in contact and responds as a linear spring. As
59
the normal force becomes positive, contact is broken and no force is
transmitted (unless KEYSUB(1 )*1 , then a small force is supplied to
prevent a portion of the structure from being isolated).
In the tangential direction, for F < Q and the absolute value of
the tangential force (F ) less than or equal to (u F ), the interface
x y
does not slide and responds as a linear spring in the tangential direc
tion. However, for F < and F > u F , sliding occurs . Note that
y x y
F v is a variable and if contact is broken, the tangential function
A
degenerates to a zero slope straight line through the origin (or of
slope k/10 5 , if KEYSUBOH ) indicating that no (or little) tangential
force is required to produce sliding. Figure 5.10 shows the displace
ment functions for this element.
Assumptions and Restrictions . The gap interference is specified
independent of the nodal point locations. Nodes I and J may be coin
cident since the orientation of the interface plane is defined only by
the angle 8. The element is defined such that a positive normal dis
placement (in the element coordinate system) of node J relative to
node I tends to open the gap, as shown in Fig. 5.9. If, for a given
set of conditions, nodes I and J are interchanged, or if the interface
is rotated 8 + 180°, the gap element appears to act as a hook element,
i.e., the gap closes as the nodes separata. The element may have
rotated nodal coordinates since a displacement transformation into the
element coordinate system is included.
The friction coefficient is evaluated at the average of the two
node temperatures. The twodimensional interface element must be de
fined in an XY plane and the global X axis must be the radial direc
tion for axi symmetric problems. The element operates only in the
Static (K20=0) and the Nonlinear Transient Dynamic (K20=4) analyses.
If used in other analysis types, the element maintains its initial
status throughout the analysis. Note, a gap condition capability is
also included in the Reduced Linear Transient Dynamic (K20=5) Analysis.
No moment effects are included due to nodal points offset from a
line perpendicular to the interface. If INTERFERENCE is zero (or
blank), the element stiffness is included in the first iteration, un
less START = 3.0. The element requires an iterative solution with
the stiffness matrix reformulated each iteration. Note that if the
element status changes within an iteration, the effect of the changed
status is included in the neat iteration nonconverged iterations are
not in equilibrium.
70
TABLE 5.1
ELEMENT SUMMARY 7A3LE
STIfFMgSS
NO.
NAHg
6
a
9
10
1 1
12
13
u
13
16
17
la
19
20
21
22
23
2*
25
26
27
23
29
30
31
32
23
34
35
36
37
33
39
^0
3?AP, 20
CONSTANT STRAIN .ELEH .
ELST'C 3EAM, 23
ELASTIC 5EAM. 33
ELASTIC SOLID (C3T)
SLAS "LA7 TRI. PLATE
S?AR» 30
ELASTIC STRAIGHT PIPE
CA3LE
AXlSYM. CONICAL SMELL
INTERFACE ElEM. (201
EL if FLAT TPT. SMELL
S?RINGDAMP£R
MASS WITH PqTaRY INER.
MASS* 20
MASS* 30
SPRING* 20
OAMPEP » 20
PLASTIC STRAIGHT PIPE
GENERAL M^ss
COPE SPACED ANO GAP
PLASTIC 3EAM, 20
TOPS ION 5PRING0A.MPEP
AXIS?*. HARMONIC QUAD.
PLAS. FLAT 7RI. PLATE
STIFF, DAMP, "A55 MATRIX
PL FLAT SMELL (3 TEMP)
CURVED PIPE (EL30VO
CONDUCTING SOLID
RADIATION LINK
CONDUCTING 3AR, 20
CONDUCTING pap, 30
CONVECTION L INK
LINEAR TEMPER. EL.
NOUCTANCE
>ci I
HYO° iULlC
CONQUC'I^G FLAT SH;
FLUID COUPLING
SLIDING INTERFACE
COM3 InaT ION ELEVEN 
OIH.
2
I
2
3
3
2
3
3
3
2
2
3
2>3
2
2
3
2
?
3
2>3
2
2
3
2
2
3
3
3
3
2 OH
2
3
2 OR
2
OP
3
OR
OP
OR
OOF NODES TYPE
2
3»A
2
2
A»6»3
3
2
2
2
2
2
3
2
1
1
1
2
2
2
1
2
2
2
A
3
2
3
3
At 6 »3
2
2
2
2
3*4
2
3
2
2
2
PLASTIC
PLASTIC
LINEAR
LINEAR
LINEAR
LINEAR
PLASTIC
LINEAR
NONLIN
LINEAR
NONLIN
LINEAR
LINEAR
LINEAR
LINEAR
LINEAR
LINEAR
LINEAR
PLASTIC
LINEAR
NONLIN
PLASTIC
LINEAR
LINEAR
PLASTIC
LINEAR
PLASTIC
LINEAR
LINEAR
NONLIN
LINEAR
LINEAR
LINEAR
LINEAR
NONLIN
LINEAR
LINEAR
NO N LIN
NONLIN
USE STIF21
USE
USE
USE
USE
STIF21
3TIF21
5TIF1A
STIFIA
USE STIF14
USE STIFiQ
(CONTINUED ON NEXT PAGE)
71
"A8LE
I (CONTINUED)
ST IF r nESS
MO
NAME
OI».
DOF
NOOES TYPE
4i 3—3 ELAS..CUAO. MEMS.
42 LINEAR STRAIN I3QPAP.
43 EL AS FLAT PECT. SHELL
4A, TiPEPED UNSYM.. SEAM
43 ISOPARAMETRIC SOLID
46 ELAS. PLAT PECT. PLATE
47 TSANSV.HT.CCNO. SHELL 2
43 PL. PLAT SHELL !S TEH?)
49 PLASTIC SOLID
50 SU?EPEL£H£NT
32 INTERFACE ELS*. (30)
53 LAMINATED 5HELL
54,. TAPER. UNSYM. SEAM (20)
53 ISCPAP.QUAO.TEHP.ELEM
56 FLUID FLHT TRANS PIPE
57 ISO. QUAD. SHELL TEMP.
53 PLASTIC HINGE ELEM.
59 IMMERSED PIPE ELEM.
60 PLASTIC EL50W
61 A^IS7H. HARMONIC SHELL
62 20 WAVE ELEMENT
63 ELAS. "LaT CUaO. SHELL
65 30 *AYE ELEMENT
66 TPANS. THEPMfLOW PIPE
67 HT TPANSELECTPIC CUAO
63 HT TPANSELECTPIC LINE
69 HT TPANELECTPIC SOLID
70 ISO, CONOUCTING SOLID
71 LUMPED 7HEPMA>_ MASS 2
73 AXISY HARMONIC TEMP EL
3
3
4
LINEAR
2
2
4
PLASTIC
3
6
4
LINEAR
3
6
3
LINEAR
3
3
3
PLASTIC
2
3
4
LINEAR
OP 2
1
5
LINEAR
3
6
3
PLASTIC
3
3
4.6.3
PLASTIC
3
•

LINEAR
3
3
2
NONLIN
3
6
3
LINEAR
2
3
2
LINEAR
2
I
4
LINEAR
3
2
2
NONLIN
3
1
4
LINEAR
3
6
2
NONLIN
3
6
2
LINEAR
3
6
3
PLASTIC
2
4
2
LINEAR
2
2
4
LINEAR
3
6
4
LINEAR
3
2
3
LINEAR
3
2
2
NONLIN
2
2
4
ITERATIVE
3
2
2
ITERATIVE
3
2
3
ITERATIVE
3
1
3
LINEAR
CP 3
1
1
LINEAR
2
1
4
LINEAR
72
Table 5.2. Input of Element Parameters on
ANSYS Program Data Cards
Input
Element Parameter
on Card
NODS NUMBERS
El
REAL CONSTANTS
02 or E2
TEMPERATURES, FLUENCES
Q.
•PRESSURES
P
HEAT GENERATION RATES
a
CONVECTION SURFACES
P
MATERIAL PROPERTY EQUATIONS
H
KEYSU8(N)
Table 5.3. Units of Input and Output Parameters
Input Parameter Un i ts
Area L 2
Volume \?
Pressure F/L
Moment of Inertia L
Fluence (?t) Neutrons/L
Density M/l 3
Convection Coefficient Q/L tT
Conduct i vi ty Q/LtT
Specific Heat Q/MT
Heat Generation Rate Q/l t
(except for STIF71 ) (Q/t)
Spring Constant F/L
Damping Coefficient Ft/L
2
Rotational Inertia F^t
2
Output Parameters Units
Stress F/L 2
Strain
Moment or Torque LF
Twist Radians
Heat Flow Rate Q/t
74
TA3LE 5.4.
ISOPARAMETRIC SOLID ELEMENT  THREE IMENSIONAL
SUSPOUTINE NAM£
NO. C. c NODES PER ELEMENT
DEGREES Or FacZOQH ?€5? NOCE
R£<3UTfi£0 REL CONSTANTS
TEMPERATURES
PRESSURES
MATERIAL PROPERTY EOUATIONS
MATRTCES CALCULATED
PLASTICITY
CREEP ANO SWELLING
FORCES SAVED ON TAPE
KEYSU3U)
KEYSuS(lA)
KEYSU3(13>
STIFFS
a
3
3
6
I»J»KtL»M,N»0»P
UX.UYtUZ
10
TCI) »T(J) ,T<K) ,T(L) »T(H) ,7(N) »
T(O) ,T(P)
P(IJXL) jP (IJNM) ,P(JKON) ,?(KLPO) ,
P(LIMP) »P(NHCP)
EX ♦ EY , EZ y ALPX » ALPY , Al_PZ >
NUXY ,NUTZ >NUXZ » OENS .
GXY*GYZ>GXZ (OPTIONAL)
HASSt STIFFNESS
YES
NO
 GENERAL 30 APPLICATION
1  GENERALIZED PLANE STRAIN OPTION
 USE 3X3X3 LATTICE CF INTEGRATION POIN
(USED FOR INCREASED ACCURACY WITH
WARPED ELEMENTS ANO ELEMENTS HAVING
HIGHLY NONRECTANGULAR SHAPES)
1  USE 2X2X2 LATTICE OF INTEGRATION POIN
(KEYSUS(IA) IS INTERNALLY SET TO 1 F
PLASTICITY SOLUTIONS)
 DISPLACEMENT FORMULATION INCLUDES Th.E
EXTRA HOOE SHAPES
1  DISPLACEMENT FORMULATION OOES NOT
INCLUDE THE EXTRA MODE 5HAPE5
(CONTINUED ON NEXT PAGE)
75
TA8LE 5.4 (CONTINUED)
XEYSU3(2) C  NO SURFACE STRESS OUTPUT
1  PRINT GUT STRESSES FOR SURFACE 2
2  PRINT GUT STRESSES FOR 5GTK SURFACES
2 AiNO ;
(SURFACE STRESSES AVAILABLE FOR
ISOTROPIC, ELASTIC MATERIALS ONLY)
3  PRINT GUT SOLUTION AT EACH INTEGRATION
POINT AS WELL AS AT CSNTROIO
(FOR PLASTICI7C SOLUTIONS ONLY.
NOTE  AOOS 21 MORE LIMES ? c 3 SLZ&EIT)
3  PRINT STRESSES AT THE 3 NODES AS WELL
AS AT CSNTROID
SUBROUTINE GATE V 30/72
X V I T * XXXXXXXXX ** 9' M X M . T M ■ ? W W X ' J F X » ■ • M ^t f H^I A M A A A A * A A ■ ' X ' J J TT » W J f M. X X  ■ M
76
TABLE 3.5
ISOPARAMETRIC SOLID ELEMENT  THREE OIMSNSIONAL
EL£M£?*T PRINTOUT EXPLANATIONS
EXPLANATION
LAoEL
NUMBS?.
C3NSTA^
0?
ITS
FOP MAT
LINE 1
SQL in
NOOSS
xc»rc»2C
TEMP
1
a
3
1
15
ais
3F3.3
F5.0
LINE 2
EPS
6
6F9.6
SIG
6
6F3.<3
LINE 3
SIGPo
TAUMaX
EP?R
VOL
VM
3
i
3
1
1
3F3.0
F7.0
3F9.6
F12.3
F3.0
ELEMENT NUMBER
MOOES I>J>K,L»H,N,0»P
X,Y,Z COORD I?JAT£3 OF ELEMENT CcNTROID
ELEMENT AVERAGE TEMPERATURE
E?X»E?Y,E?Z>GAMMAXY»GAMMAYZ»GAHMAX2 (GLOBAL
(ELASTIC STRAIN COMPONENTS)
SIGX»SIGY»5IGZ>TAUXY>7AUYZ>TAUXZ (GLOBAL J
PRINCIPAL STRESSES SIG1 ,S IG2 >SIGD
MAXIMUM S'ritM^ STRESS
PRINCIPAL STRAINS ER1 , E?2 . E?3 (ISOTRCPIC
ELEMENT VOLUME
VON MI3ES EOUIVALENT STRESS
LINE IJNM SURFACE 2 STRESS CONDITIONS (PRINTED ONLY IF x£YSUS<2) IS
GREATSp THAN ZERO)
SURFACE AREA
AVERAGE SURFACE TEMPERATURE
SIGX» SIGYt AND TAUXY
(X AXIS PARALLEL TO TM£ AVERAGE Or LINES
I J ANO MN)
VMS 1 F3.0 VON MISES EOUIVALENT STRESS FOR THIS FACE
LINE IJNM SURFACE 2 STRESS CONDITIONS (CONTINUED)
MAXIMUM* MINUMUM* ANO MAXIMUM SMEaR STRESS
ON SURFACE 2 OF THIS ELEMENT
ANGLE OF PRINCIPAL STRESSES (MEASURED FROM
LOCAL X TOWAflO LOCAL Y)
EPSX. E?SY, ANO GAMMAAY
SURFACE PRESSURE
(CONTINUED ON NEXT PAGE)
AREA
1
F10.A
TEMP
1
F<9.0
XY STR
3
3F3.0
HAXMlN STR
3
3F3.0
A
1
F5.1
STRAINS
PRESSURE
3
1
3F9.Q
~ Fa.o
77
TA6LE 5.5 (CONTINUED)
LINES KL?0 SURFACE <* STRESS CONDITIONS (PRINTED ONLY IF" *SYSUS(2) = 2)
(SAME AS SURFACE 2 OUTPUT 3UT APPLIED To SURFACE <*>
LINES 4 ANO 5 NONHINEAS SOLUTION (PRINTED ONLY IF K13 IS GREATER THAN
ZERO ON CAPO CD
SRPLAV 6 6F10.7 AVERAGE PLASTIC STRAINS AT CENTROIO
(X*Y,Z»XY,YZ>*Z)
SPORiV 6 6F10.7 AVERAGE ORIGIN SHIFT STRAINS AT CENTROIO'
LINE 6 NONLINEAR SOLUTION (CONTINUED)
EPGNAV I FI0.7 AVERAGE GENERALIZED STRAIN AT CENTROIO
ROSGAV 1 F1Q.4 AVERAGE GENERALIZED POISSONS RATIO
AT CENTROIO
SIGEiV 1 F10.2 AVERAGE EQUIVALENT STRESS AT CENTROIO
NOTE  STRESSES ANO STRAINS ARE PRINTED A?TER THE PLASTICITY CORRECTIONS.
78
TABLE 5.3
INTERFACE ELEMENT  T iREEOIMENSlCNAL
SUBROUTINE NAME STIF3E
NO. Or NODES PER ELEMENT 2 I>o
0EGPEE"S OF FREEDOM P*R NOOE 3 UX»UY»UZ
REQUIRED SEAL CONSTANTS 3 STIFFNESS >GAP , START
A NEGATIVE GAP ASSUMES A.N INITIAL
INTERFERENCE CONDITION
IF START = 0.0 OP BLANK, PREVIOUS STA
OF ELEMENT DETERMINED FROM GAP INPUT
IF STAPT = l.Ot GAP PREVIOUSLY CLOSED
. AND NOT SLIDING
IF STAPT =2.0* GAP PREVIOUSLY CLOSED
AND SLIDING
IF STAPT * 3.0* GAP PREVIOUSLY OPEN
TEMPERATURES Z T(I)»T(J)
PPESSijRES
MATERIAL PROPERTY EQUATIONS 1 HU
MATRICES CALCULATED STIFFNESS
PLA5TICITY NO
NON'INER YES (ITERATIVE SoL'JTIcn REQUIRED)
FORCES SAVED ON TAPE 2 NORMAL FORCE (FN )» TANGENTIAL FGPCE(FS)
KEYSUB(l)  NO STIFFNESS ASSOCIATED WITH SEPARATED
INTERFACE
1  STIFFNESS»1.0E6 ASSOCIATED WITH
SEPARATED INTERFACE FOR NORMAL MOTION
ANO WITH SLIOING INTERFACE FOR
TANGENTIAL MOTION
XEYSUP<2)  CONVERGENCE BASED ON UNCHANGING GAP STATU
1  CONVERGENCE 3ASED ON CHANGING GAP STATUS
WITHIN A 5 PERCENT UNCERTAINTY ON MU"
2  CONVERGENCE BASED ON CHANGING GAP STATUS
WITHIN A 10 PERCENT UNCERTAINTY CN VU
SUBROUTINE OATE 5/30/7D
79
TA3LE 5.7
INTERFACE ELEMENT  THREEDIMENSIONAL
ELEMENT PP1N7CUT EXPLANATIONS
NUM9EP OF
LASEL CONSTANTS FORMAT EXPLANATION
LINE i
30 GiP 1 15 ELEMENT NUHSSP
H03£5 2 2 IS NODES I AND J
USE?»USLICECY,Z) 2 2F9.3 GAP SIZE. SLIDING CISTA.NCE IN LOCAL
QIRECTTON» SLIDING DISTANCE IN L'OC
Z OIRECTION
KTY?5 1 12 INTERFACE CONDITION INOICATOP
1  RIGID CONTACT
2  SLIDING CONTACT
3  FREE
KOLD 1 12 XTYPE VALUE OF THE PREVIOUS ITEPATIC
LINE" ?
FN 1 G14.6 NORMAL FORCE (ALCNo IJ LIME)
F3 1 G14.6 TANGENTIAL FORCE (VECTOP SUM)
80
TABLE s.3
ISOPARAMETRIC QUAOPILATEPAL TEMPERATURE ELEMENT
SU3P0UTINE NAME STIF35
NO. Or MOOES PEP ELEMENT  I»J»K,L
DECREES GF FREEDOM PEP MOOS 1 TEMP
REQUIRED REAfc CONSTANTS
HEAT GENERATION RATES 1 AVERAGE
CONVECTION SUP?" ACES ^ lJ»UX,.<L»Ll
HA7E.PIAL PROPERTY ECUA7I0NS ^ XXX»KYY »OENS»C CGLC8AL)
MATRICES CALCULATED CONDUCTIVITY, SPECIFIC HEAT
KEYSU3<1>  PLANE
1  AXISYMMETPIC
«EYSu3(lA)  INCLUDE EXT* A 7EHPEPA7URS SHAPES
1  SUPPRESS E~7RA TEMPERATURE SHAPES
KEYSUS(2:  NO CONVECTION SURFACE PRINTOUT
1  PRINT OUT HEAT FLOW SATE FRO*
CONVECTION SURFACES
SVJSPOUTINE 0A7E 6/22/73
7A8LE 5.9
ISOPARAMETRIC GUACRILATERAL TEMPERATURE ELEMENT
ELEMENT PRINTOUT EXPLANATIONS
NUMBER OF
LABEL CONSTANTS FORMAT EXPLANATION
LINE i _ (PRINTED ONLY IF K£YSUS(2) = 1)
ELEMENT NUMBER
CONVECTION FACE NOOES
(I»J OR J*K OR ,K,L OR L»I)
CONVECTION ACE NUMBER
CONVECTION SURFACE AREA
AVERAGE FACE TEMP, FLUID SULK TEMP.
HEAT FLOW RATE ACROSS FACE
LINES 2>2» (SAME AS ABOVE FOR OTHER CONVECTION SURFACES* IF DEFINED)
ELEMENT
NOOES
1
2
15
2IS
FACE
AREA
12
Fa.*
TAVG.T3ULX
HEAT FLOW
2
1
2F6.0
Gil. A
81
TABLE 5.10
CONDUCTING BAR  TWODIMENSIONAL
SUBROUTINE NAME
NO. OF NODES PER ELEMENT
DEGPEES OF FREEDOM PER NODE
REQUIRED REAL CONSTANTS
HEAT GENERATION ,RATES
CONVECTION SURFACES
MATERIAL PROPERTY EQUATIONS
•MATRICES CALCULATED
ELEMENT PRINTOUT
SUBROUTINE OATE
ST
IF32
2
I,J
1
TEMP
1
AREA
1
AVERAGE
3
KXX.DENS.C
CONDUCTIVITY .SPECIFIC
HEAT
NONE
7/'
01/70
p M x M' 'A' 'X X' 'X 'Jfc *X J
82
TABLE 5.11
TViO— DIMENSIONAL ISGPaflAHETRlC ELEMENT
SUBROUTINE NAM?
NO. OF NODES PES ELEMENT
DEGREES 05" FREEDOM PER N02E
REQUIRED PEAL CONSTANTS
TENPFPATUnES
PRESSURES
MATERIAL PROPERTY EQUATIONS
MATRICES CALCULATED
PLASTICITY
CREEP AND SWELLING
FORCES SAVED CN TAPE
KEYSua CD
KETSuBClAJ
STIFLE
2
1
6
10
I»J*X»L (NUMBER CCUNTERCLQCXylSE)
UX*UY
IF" KSYSUS(l) = 0.1.2
THlCXNESS, IF XSYSU3U) » 3
Til) ,TU> ,T(X) »T(L)
PCI) »P<2> *P<3) »P(*)
IF PLANE STRESS 
EX ,SY .NUXY , AL?X , AL?Y ,OENS
GXY (OPTIONAL)
IF AXISYM OR PLANE STRAIN 
EX,EY»E2,.NUXY,NUY2.NUX2»AL?X,ALPY>
ALP2»0ENS GXY (OPTICNAL)
MASS ♦STIFFNESS
YES
NO
26
SIGMAX.SlGMIN.TAUMAX.SIG2.SIGc.
E?GSN»SIGX.S I GY,TAUXY. TEMPERATURE.
W ELASTIC STRAINS, \ PLASTIC STRAI
4 0. SHIFT STRAINS, 4 THERMaL STRaI
 PLANE STRESS
1  AXISYHMETRIC
2  PLANE STRAIN (2 STRAIN = 0.0)
3  PLASZ STRESS WITH THICKNESS INPUT
 DISPLACEMENT FORMULATION INCLUDES THE
EXTRA MOOE SHAPES
1  DISPLACEMENT FORMULATION DOES NOT
INCLUOE THE EXTRA MOOE SHAPES
(CONTINUED ON NEXT PAGE)
83
TABLE 5. IT
(CONTINUED)
<£YSuS(2}
3 
t+ 
NO SURFACE STRE33 PRINTOUT
PRINT OUT STRESSES FOR SURFACE I J
PRINT OUT STRESSES FOR 30TH SURFACES
I J AND KL
(SURFACE STRE33 PRINTOUT AVAILABLE ONLY
FOR ISOTROPIC. ELASTIC MATERIALS)
PRINT OUT SOLUTION AT ALL INTEGRATION
POINTS AS WELL AS AT CZNTROID (FOR
PLASTIC SOLUTIONS ONLY. ADOS 15 MORE
LINES ?Z? ELEMENT")
PRINT STRESSES AT Th£ <+ NODES AS WELL
AS AT CSNTROID (KEYSU8QA) MUST = 0)
*£T5u3(2A)
 PRINT SOLUTION A7 ELE.ME.NT CcNTROlD
1  REPEAT LINES 1 ANO 2 OF SOLUTION FOR
ALL OTHER INTEGRATION POINTS (ACOS
16 MORE LIN 13 PZri ELEMENT 1
SUBROUTINE OATE.
^/DO/72
34
TAfcLE 3.12
t'wooi^ensicnal isoparametric et.shs.nj
element printout explanations
LAS£L
NUHSE.R OF
CONS 7 AN 7 3
FORMA 7
line i
EL EM
NODES
vol
MA7EP I A
STRESS
S 1 3 E.~F
L
IM"
1
4^
i
1
1
I
15
415
"1 .A.
12
"3.0
F3.0
LINE 2
X
Y
i
XY 3TR
I
1
1
4.
F6.2
F6.2
F5.0
4F 3 • 0
H.A^T»I*N
1 S7
R 3
3F3.0
A
1
F5.1
EXPLANATION
ELEMENT NUM5SR
N00S3 I* J, X, A.NO L
VOLUME Of ELEMENT
MATERIAL NUM9ER
STRESS INTENSITY IN THIS ELEMENT
VON MIScS EQUIVALENT STRESS
X. COORDINATE C? CENTROID OF ELEMENT
Y C00R0INA7E Or CENTpOID OF ELEMENT
AVERAGE 7EHPERAuRE OF ELEMENT
SIGx, SIGY, TAUxY. NO SIGZ
(SIG2=0.0 FOR PLANE STPE3S ELEMENTS)
3IGHAX, SIGN IN, ANO TAUMAX
(INPLANE PRINCIPAL STR£SS£3)
ANGLE OF PRINCIPAL STRESSES RESTIVE TO
7h£ GL03AL XY ±ZZ5
LINE I J SURFACE I J STRESS CONDITIONS (PRINTED ONLY. IF KEYSU3<2> IS
1 OR 2)
AVERAGE TEMPERATURE OF IJ SURFACE
ELASTIC SURFACE STRAIN COMPONENTS
(PARALLEL* PERPENDICULAR* Z OR HOOP)
ELASTIC SURFACE STRESS COMPONENTS
(PARALLEL* PERPENDICULAR* Z OR HOOP}
SURFACE STRESS INTENSITY, SU^f XCZ
VON MISE5 EQUIVALENT STRESS
LINE XL SURFACE XL STRESS CONDITIONS (PRINTED ONLY IF x£YSUS(2) = 2)
tSAHE AS LINE IJ.ASQVE 3UT APPLIED TO FACE XD
LINES 3 ANO 4 NONLINEAR SOLUTION (PRINTED ONLY IF X13 IS GREATER THAN
ZERO ON CARD CI)
£?SL 4 4F10.7 ELASTIC STRAIN COMPONENTS CX,Y,XY,Z)
EPPL  4 4F10.7 PLASTIC STRAIN COMPONENTS (X,Y,XY,Z)
LINE 3 NONLINEAR SOLUTION (CONTINUED)
eporig 4 4f10.7 shift of origin of stressstrain curve due
70 Previous loao cycles
spgen 1 f10.7 equivalent strain
PC5G£N 1 F10«A EFFECTIVE P0ISS0NS RA7I0
SIGE 1 F10.2 EQUIVALENT STRESS
NOTE I  STRESSES AND STRAINS ARE PRINTED AFTER THE PLASTICITY CORRECTIONS.
NOTE 2  FOR AXlSYNMETRIC SOLUTIONS, THE X,Y,XY» AND Z STRESS ANO STRAIN
OUTPUTS CORRESPOND TO THE RAOIAL, AXIAL, INPLANE SHEAR * AND HOOP
STRESSES ANO STRAINS, RESPECTIVELY.
T
STRAIN
1
3
F3.0
3F10.7
STRESS
3
3F3.0
2
2F9.0
35
TABLE 5.13
INTERFACE ELEMENT  TJQ DIMENSIONAL
SUBROUTINE NAME
NO. OF NOOSS PZri ELEMENT
CEGREE3 0?" rS£S30H PER NOQE
REQUIRED REAL CONSTANTS
TEMPERATURES
P PES SUP £3
MATERIAL PROPERTY EQUATIONS
MATRICES CALCULATED
PLASTICITY
FCRCFS SAVED ON TAPE
KEYSU8<1>
<EYSti8<2)
STIF12
2
2
I.J
UX»U7
TH£TA*STIFFNESS* INTERFERENCE* START.
A NEGATIVE INTERFERENCE ASSUMES AN
INITIALLY OPEN GAP
IT START = 0.0 OR 5LANX, PREVIOUS
CONDITION CF SAP DETERMINED FROM
INTERFERENCE
IF START = 1.0* GAP PREVIOUSLY CLOS
ANO NOT SLIDING
IF START = 2.0. GAP PREVIOUSLY CLOS
AND SLIDING RIGHT
IF START => 2.0 » GAP PREVIOUSLY
CLOSED ANO SLIDING LEFT
IF START = 3.0» GAP PREVIOUSLY OPEN
T(I) ,T(J)
HU
SUBROUTINE DATE
STIFFNESS
NO (NONLINEAR ELEMENT)
2 NORMAL FORCE(FN)» TANGENTIAL FORCECF
 NO STIFFNE35 ASSOCIATED WITH SEPARATED
INTERFACE
1  STIFFNESS»I.0E<5 ASSOCIATED WITH
NORMAL STIFFNESS FOR SEPARATED INTER
FA.CZS AND WITH TANGENTIAL STIFFNESS
FOR SLIDING INTERFACES
 CONVERGENCE 3ASED ON UNCHANGING ElEME>
STATUS
1  CONVERGENCE BASED ON CHANGING ELEMENT
STATUS WITHIN A 5 PERCENT TOLERANCE C
HU
2  CONVERGENCE 3ASED ON CHANGING ELEMENT
STATUS WITHIN A 10 PERCENT TOLERANCE
MU
<*/0W72
86
TASLE 5.14
INTERFACE. ELEMENT  TWO DIMENSIONAL
. ELEMENT PRINTOUT EXPLANATIONS
EXPLANATION
ELEMENT NUH3E5?
NOOES I ANO J
GAP SIZE* SLIDING DISTANCE
NORMAL FORCE
TANGENTIAL FORCE
ELEMENT STATUS
1  GAP CLOSED, NO SLIDING
2  SLIDING CONTACT (NOOE J MOVING TO
RIGHT Or NOOE I)
2  SLIDING CONTACT (NCOS J MOVING TO
LEFT OF NOOE I)
3  GAP OPEN
OLD 1 12 KlyPE VALUE" OF THE PREVIOUS ITERATION
NUH8ER
OF
LA3FL
csnsta.s
iTS
FORMAT
EL EM
1
15
NQOE5
2
2IS
US£?,USLIDE 2
2F9.S
FN
1
G13.5
FS
1
G13.5
KTYPE
1
12
87
z
I
^— Y
MOTE  Surface stressas ara available on faces 2 and 4.
(Surface coordinate system shewn)
Figure 5.1. Three Dimensional Isoparametric Solid Element
Z
M
Figure 5.2. ThreeDimensional Isoparametric Solid Element Output
88
Figure 5.3. ThreeDimensional Interface Element.
>
I
F n
Slope = k/10 6
if KEYSX3B(1)=1
. ■
A*
( u n)j< u n)l + ' GAP
/i
"IN
Slope=k/lO
or* KEYSUB(l)=l
T
±5% tolerance
if KEYSUB(2)=1
>•
(usJj^sJj  USLIDE
^I F «i
for F <
n
Figure 5.4. ThreeDimensional Interface Element Output
89
(or Axial )
Q  Convection Face Numbers
Heat flow out of the element is positive
(or Radial)
Figure 5.5. Isoparametric Quadrilateral Temperature Element
90
(or Axial )
>— X (or Radial)
Figure 5.6. TwoDimensional Conducting Ear Element
91
( or Axial
£\  Face Numbers
Surface Stresses are
available on Face 1
and Face 3.
X (or Radial)
Figure 5. 7 . Two Dimensional Isoparametric Element
(or Axial)
t*— X (or Radial)
Figure 5.3. TwoDimensional Isoparametric Element Output
92
Y
ar Axial)
I
INTERFERENCE CONDITIONS I
I *■
8 determines element
orientation
I * T(I)
Nodes may be coincident
(or Radial)
■£ 1 5 »'
S<°
+= •— o
*}s>oh
RIGHT SLIDE
(KTYPE OR START
= +2)
Figure 5.9. TwoDimensional Interface Element
SLOPE = k/10 6
IF KEYSUB(1)=1
c*,j.<«v,) x j
Fl
SLOPE = k/10
IF KEYSUBI
iYSUB(l)=l 2
Cu,l Cu,) x 
usuioe
 M\F^ (
For F« < O
Figure 5.10. Two Dimensional Interface Element Output
93
CHAPTER 6
CONCLUSION
The manual for ANSYS for analysts of anchored pavements has been
prepared to provide the user a ready reference for analyzing the re
sponse of anchored pavement system subjected to vehicle static loads,
moisture variation, and temperature variations.
The manual is prepared so that it can be used with a minimum num
ber of references. For preprocessing, Chapter 3 provides the details
of a program developed at I IT called FEMESH. The User's Guide for
ANSYS has its own preprocessing subroutines, however, the FEMESH is
more efficient for preprocessing the anchored pavement system. If any
postprocessing Cpostplotting) is desired, the User's Guide for ANSYS
should be consulted. In the particular analysis performed, postpro
cessing was not utilized as plotting was done by hand.
The computer program provides the numerical values of stresses,
strains, deflections in all elements of various materials. There is
no practical limit of restriction of material numbers, that is the
program can be used with different materials in any direction. For
heat transfer, the program provides the distribution of temperature
versus time at any point.
ANSYS in general has the capability of obtaining response of the
pavement system under transient dynamic loads, however, this has not
been incorporated in this manual.
The most noteworthy point for the ANSYS program is the wave front
solution and certain limitations caused by the said solution. The
ordering of nodes therefore must be done to minimize the size of wave
front as has been explained in detail in Chapter 4. The program has
been found versatile and capable of solving complex geometrical struc
tures resting on complex geologically earth mass.
94
REFERENCES
1. Bathe, K.J. and Wilson, E. L. , "Numerical Methods in Finite
Element Analysis," PrenticeHall, Inc., (New Jersey, 1976.
2. Cook, R. 0., "Concepts and Applications of Finite Element
Analysis," John Wiley and Sons, New York, 1974.
3. Desai, C. S. and Abel , J. F, , "Introduction to the Finite
Element Method," Von Nostrand Company, New York, 1972.
4. DeSalvo, G. J., "ANSYS Verification Manual," Swanson Systems
Inc., 1976.
5. DeSalvo, G. J. and Kohnke, P. C. , "ANSYS Introductory Manual,"
Swanson Analysis Systems Inc., 1975.
6. DeSalvo, G. J. and Swanson, J. A., "ANSYS Examples Manual,"
Swanson Analysis Systems Inc., 1972.
7. DeSalvo, G. J. and Swanson, J. A., "ANSYS User's Manual
CRevision 2)," Swanson Analysis Systems Inc., 1975.
8. DeSalvo, G. J. and Swanson, J. A., "ANSYS User's Manual
CRevision 3)," Swanson Analysis Systems Inc., 1978.
9. FORTRAN Extended Reference Manual, Publication Mo. 60497800,
Control Data Corporation.
10. Guyan, R. J., "Reduction of Stiffness and Mass Matrices,"
AIAA Journal , Vol. 3, No. 2, Feb. 1965.
11. INTERCOM Reference Manual, Publication No. 60494600,
Control Data Corporation.
12. Irons, B. M. , "A Frontal Solution Program for Finite Element
Analysis," International Journal for Numerical Methods in
Engineering , Vol. 2, No. 1, Tan., p.p. 523, (Discussion May ,
1970, p. 149), 1970.
13. Jones Jr., R. F. and Costello, M. G. , "A Solution Procedure for
Nonlinear Structural Problems," . Numerical Solution of Nonlinear
Structural Problems , ASME, pp. 157169, 1973.
14. Kohnke, P. C. , "ANSYS Theoretical Manual," Swanson Analysis.
Systems Inc. , 1977.
15. Kohnke, P. C. and Swanson, J. A., "ThermoElectric Finite Elements,"
International Conference on Numerical Methods in Electrical and
Magnetic Field Problems, Santa Margherita Ligure, Italy, June 14,
1976.
95
16. Lekhnitskii, S. G. , "Theory of Elasticity of an Anisotropic
Elastic Body," Hoi denDay, San Francisco, 1963.
17. Loader Reference Manual, Publication No. 60429800, Control
Data. Corporation.
18. Melosh, R. J. and Bamford, R„ M. , ''Efficient Solution of
LoadDeflection Equations," Journal of the Structural Division ,
ASCE, Vol. 95, No. ST4, Proc. Paper 6510, pp. 661676,
CDiscussions, Dec. 1976, Jan., Feb., May 1970, Closure Fed.
1971), April 1969.
19. NOS/BE Reference Manual, Publication No. 60493800, Control
Data Corporation.
20. NOS/BE Users Guide, Publication No. 60494000, Control Data
Corporation.
21. Przemieniecki , J. S., "Theory of Matrix Structural Analysis,"
McGrawHill, 1968.
22. Ralston, A. and Wilf, H. S., "Mathematical Methods for Digital
Computers," John Wiley & Sons Inc., New York, 1962.
23. UPDATE Reference Manual, Publication No. 60449900, Control
Data Corporation.
24. Wilson, E. L. , Taylor, R. L. , Doherty, W. P., and Ghaboussi, J.,
"Incompatible Displacement Models," Numerical and Computer
Methods in Structural Mechanics , Edited by S. J. Fenves, et al . ,
Academic Press Inc., New York and London, pp. 4357, 1973.
25. Zienkiewicz, 0. C. , "The Finite Element Method in Engineering
Science," McGrawHill Company, London, 1971.
96
APPENDIX A
NOTATION
The notation defined below is used throughout the appendices B and C.
General
Tzrzi Meaning
[3] Straindisplacement matrix
[C],[CJ Damping matrix, thermal damping matrix
[D] Stressstrain matrix
E Young's modulus
{F} Force vector
[K],[K] Stiffness matrix, conductivity matrix
[H] Mass matrix
{Q} Heat flow vector
{T> Temperature vector
[T R ] Local to global conversion matrix
u,v,w,{u} Displacement, displacement vector
dtl Virtual internal work
6V Virtual external work
x,y,z Element coordinates
X,Y,Z Nodal coordinates (usually global cartesian)
a Coefficient of thermal expansion
z Strain
v Poisson's ratio
c Stress
97
Superscripts and Subscripts on [ML ("CL'TO, (u>, {T}, and/or (F)
No subscript implies the total matrix in final form, ready for solu
ti on .
a nodal effects caused by an acceleration field
c convection surface
cr creep
e based on element in nodal coordinates
g internal heat generation
l based on element in element coordinates
Id large displacement
m master
n nodal effects caused by externally applied loads
pi plasticity
pr pressure
s slave
sw swelling
t thermal
— (bar over term) heat transfer matrices
(flex over term) reduced matrices and vectors
(dot over term) time derivative
98
APPENDIX 3
ANALYSIS PROCEDURES
This section of the manual is designed to give users an understanding
of the theoretical basis of each analysis type. The derivation of the individual
element matrices and vectors is discussed in Appendix C.
In the matrix displacement method of analysis based upon finite element
idealization, the structure being analyzed must be approximated as an assembly
of discrete structural elements connected at a finite number of points (called
nodal points). If the forcedisplacement relationship for each of these dis
crete structural elements is known (the element "stiffness matrix") then the
forcedisplacement relationship for the entire structure can be assembled using
standard matrix methods.
Figure Bl gives a summary of the ANSYS analysis procedures available
and may be used as a guide in selecting which type to use. Each of the
analysis procedures is described in the following sections.
STATIC ANALYSIS
The overall equilibrium equations for static analysis' are:
[K]{u> = {F} (B.l)'
N
where: [K]  total stiffness matrix  Z [K ]
m=l e
{u} = nodal displacement vector
N  number of elements
C'O = element stiffness matrix (may include
the element stress stiffness matrix^
99
f start)
TRANSIEHT AND
STEADY STATE
THERMAL ANALYSIS
SUCKLING ANALYSIS
(:<a,nt) I
NONLINEAR
TRANSIENT DYNAMIC
ANALYSIS
C<AN»<M
REDUCED LINEAR
DYNAMIC TRANSIENT
ANALYSIS
(JCANS)
HARMONIC RESPONSE
IS
(XAN3)
^ANALYSIS
REDUCED HARMONIC
RESPONSE ANALYSIS
( KAN6 )
MODE FREQUENCY
 ANALYSIS
(JCAN2)
<AN is tha '<ay input on tha CI card to select the analysis type
Quasi Linear  the only nonlinearities peraittad ara caps.
Figure Bl. Summary of ANSYS Analysis Types
100
{F}, the total force vector, is defined by:
•{F} = {F n } + (F a ) + Z ({F*}+ (Ff > + {F? 1 } + {Ff }
+ (Ff } + {Fl d » (3.2;
e a
where: {F } = applied nodal load vector
{F } = [M]{A } = acceleration load vector
N
[M] s total mass matrix 2 [M ]
m=l a
[M ]  element mass matrix
{A } = nodal acceleration vector
(FT = element thermal load vector
e
{F^ } = element pressure load vector
CF? } = element plastic strain load vector
e
{F }  element creep strain load vector
{F } = element swelling strain load vector
e
{F } = element large displacement load vector
The same definitions used here apply to all other analysis procedures except
heat transfer analysis.
If sufficient boundary conditions are specified on {u} to guarantee 2
unique solution, equation 3.1 can be solved to obtain the nodal point dis
placements at each node in the structure. The simultaneous equations with all
degrees of freedom (including those with specified displacements) are given in
equation 3.3.
101
:<
K
r
<r T
K rr
/
>
r \
F.
V
(B.3)
L J
The subscript r is associated with the reaction forces. Mote that {u }
H
is known, but not necessarily equal to {0}. The top half of equation
3.3 inay be solved Tor' lujr
{u} .= [;<] '[^{u^ + [K]"'{F}
The reaction forces {F } may then be computed from the bottom half of
equation 3'. 3 ;
(F r > » c^fcu} + [;< rr ]{u r >
(B.5)
These reaction forces should always be in equilibrium with the applied
loads. The following circumstances could cause a disequilibrium, usually
a moment disequilibrium:
1. The presence of stress stiffening
Mote that moment equilibrium is not preserved/
•"Hits may. be accounted for as as
implicit updating of the coordinates.
2. Tne presence of fournoded shell elements where the
four nodes do not lie in a flat plane.
3. The presence of nodal coupling or constraint equations.
The user can write any form of relationship between the
displacements, and these may induce fictitious forces or
moments. Thus, the reaction force printout has been used
to detect input errors.
102
1.3 HEAT TRANSFER ANALYSIS (KAN=1)
Steady stats and transient heat transfer problems may be solved by
finite element techniques analogous to those used for structural analysis.
A. Steady State
The basic thermal equilibrium equation is:
ro<T}.tQ) (B.6)
where: [K] ■ thermal conductivity matrix
CQ} = heat flow vector
{T}  vector of the nodal point temperatures
This equation is identical in form to equation B.l for static analysis.
If the material properties and film coefficients are not temp
erature dependent, equation B.6 can be solved directly with one
iteration. If the material properties (or film coefficients) are temper
ature dependent, they are evaluated at the temperature of the previous
iteration. The procedure used is shewn in Figure B2.
An optional convergence criterion is available with steady
state analysis. All nodes are monitored for the largest change in temp
erature. If this largest change is less than the criterion,, then the
solution is said to be converged. This criterion is input on the MD card
(TCV) and defaults to 1.0 degree.
103
(Stjrt)
Set all
temperatures equal
t0 T UNIF (l ' nput
quantity)
Evaluate [1] p 4
i
Solve for {7}
Figure B2.
Flow chart for Steady State Heat Transfer
Analysis with Temperature Dependent
Material Properties.
B. Transient
The basic thermal diffusion equation is:
[C]{T } + [K]{T} = {Q}
where [C] is the specific heat matrix.
(B.7)
104
The form of this equation is .identical to the nonlinear dynamic
transient equation (KAN4) except that the mass term is not present. For
temperature dependent material properties (or film coefficients), the eval
uation of the properties is made at a temperature extrapolated from the
previously calculated temperatures.
The timeintegration schemes are also the same as that of the non
linear transient dynamic analysis type (KAN=4) except that the options
offered are one order lower, i.e., linear (KAY(2)=2) and quadratic (KAY(2)=0
or 1, the recommended usage). The linear (first order) equation is:
(^[C] +'TO){T t > = {Q(t)> + CC]{T t1 ) ^ (B.3)
The quadratic (second order) equation is:
(
2At n + At, t
St^^Cc] + raja t > = (Q(t) ) +
where: t Q ■ present time
t, = previous time
t~ = time at second previous time
At,  V fc 2
T, ■ temperature at this time step (to be calculated)
T. , = temperature at previous time step (known)
T t 7  temperature at secondprevious time step (known)
105
The starting procedure of the transient thermal analysis is as
follows: If the first load step is run at time = 0. (TTME=0. on L card), a
steadystate analysis is performed at that time. Alternatively, if the first
load step is run at time > 0. (TIME > 0. on L card), all temperatures at
time = 0 are set equal to TUNIF. The temperatures at time = £, (t. means
the solution at time i) are determined by the user selected time interpret
ation procedure (linear or quadratic, depending on the value of KAY(2J). If
the quadratic integration is used, it is started by setting all temperatures
at a previous time point (t ,) to those values at time = 0.
It is not recommended that the time step size between adjacent
d 2 J
iterations be changed by more than a factor of ten, unless — j is very
• dT
smal 1 .
An option is available to increase the time step size automatically
if the rate of change of temperature at all nodes is less than an input
criterion. This optimization criterion is input on the MD card as TOY, which
defaults to 5.0 degrees. Using the default value, this criterion may be
expressed as:
max
d*T ,.2
dr
< 5,
(3.10)
Because a history has to be developed, the time step size may be increased
only after the second iteration.
106
APPENDIX C
ELEMENT LIBRARY
Each element In the ANSYS program is discussed in this section. The
assumptions required to generate the element matrices and load vector are
given,, including the assumed shape functions. Certain aspects are also dis
cussed' in the chapters on the nonlinear capabilities of ANSYS. Elements with
nonlinear material properties (plasticity, creep, and/or swelling) have appro
priate quantities saved at the integration points, except as noted.
In broad terms, all stress and thermal elements have their appro
priate matrices and vectors derived using the procedures in the following two
sections entitled:
Virtual Work Derivation for Stress Analysis Elements.
Virtual Work Derivation for Thermal Analysis Elements.
These derivations assume the use of an isoparametric element* as that element
family is one of the simplest. On the other hand, a complete virtual work
derivation is also given with elements STIF46, STIF53, and STIF61 , which are
not isoparametric elements.
Virtual Work Derivation for Stress Analysis Elements .
The principle of virtual work says that a virtual (very small)
change of the internal strain energy must be offset by an identical change
in external work due to the applied loads, or:
6\J = 5 V (C.l)
where: $ u = virtual strain energy (internal work)
5 V ■ virtual (external) work
107
"he virtual strain energy is
{o} 1 {a} d(vol)
vol
(C.2)
where: {s } = strain vector
{a}  stress vector
vol = volume of element
The stress is related to the strains by:
M = [D](u>  { £th })
(C.3)
where: [D] = material property (constitutive) matrix
te+u} ~ thermal strain vector
Equation C,3 ' may also be written as
(s}= a th ) + [orV)
(C.4)
For the case of threedimensional solid elements, equation (2.0.4) may
be exoanded to:
r ~\
r ^
£ x
V T
£ y
a AT
y
S z
V _ J
a AT
Y
xy
r ~ ]
y
xy
V
At
V. /
^ J
y +
E
? r
xy xz
\  f^
E y E z
_^x ™ i Q
E y u z
; xy
1
~—
G yz
Q
1
xz
<
V (C5)
xy
'yz
T xz
108
/■/here AT  the difference at the point in question between its own temperature
and the reference (strain free) temperature (TREF).
The [D] matrix is presumed to be symmetric, so that:
J£X s _X£
E x E y
(C.fi)
ZX _ XZ
(C7)
(C.3)
Thus, in terms of ANSYS input variables:
[D]
1
1
EX
NUXY
EY
NUXZ
EZ
NUXY
EY
1
EY
NUYZ
EZ
NUXZ
EZ
NUYZ
EZ
1
EZ
1
GXY
1
GYZ
1
GXZ
(C.9)
and:
{£ th>
= <
'alpxutP
ALPY(aT)
ALPZ(aT)
>
(CIO)
109
If GXY, GYZ, and GXZ are not input, they are computed as
rvv  ^X EY (r in
Ga/ " £X + £Y + 2 NUXY EX l j
G7Z S £Y + £Z + 2 NUYZ £Y (C ' 12)
GXZ S cv , C>" ■ % UIIV7 V ( C . I 3 ,
EX + t£ + 2 NUXZ cX
A further comment on the [D] matrix: It must be positive definite.
This condition is always met if the material is isotropic or NUXY, NUYZ,
and NUXZ are all zero. But, for example, if EY is less than cr equal to
2
EX (NUXY) , the material is not positive definite.
{e ) may also be considered to include plastic, creep, and
swelling effects, where applicable.
Equations C.2 and C.3 are combined to give:
<5U = J ({6£} T [0]{£>  {o£} T [D]{ £th » d(vol) (C14)
'vol
The strains may be related to the nodal displacements by:
U>  CB]{u} (C.15
where: [B]  straindisplacement matrix
{u}  nodal displacements
Combining C.15 with C. 1 4 ., and noting that {u} does not vary
over the volume:
<5U =(u} T
[3] T [0][3j{u} d(vol)
vol
 (u} T f [3] T [0]U th } d(vol) (C.16)
vol
110
Next, the virtual work will be considered. The inertia! effects
will be studied first:
«VI {Sw^UfVvoI)} d(vol) (C.T7)
J vol
where: {w} « vector of displacements of a general point
{r } ■ acceleration (D'Alembert) force vector
According to Newton's second law.
7or = PiT {W} . «T8>
where: p  density
t ■ time
The pointwise displacements are related to the nodal displace
ments by:
w  [A] u (C.19)
where [A]  matrix of shape functions. Combining equations
C.18 and*CiT9":
5V = {5u} T p I [A] T [A] d(vol) Wu} (C20)
/vol 3t
The pressure force vector formulation starts with:
5V = I {5w} T {p} d(area) (C.21)
' area
where {p}  the applied pressure vector (normally contains only one
nonzero component).
Ill
Combining equations
5V = {6u> T f [A] T { P } d(area) (C.22)
area
Finally, equations
combined to give:
{5 a} 7 [3] T [D][3]{u> d(vol)
Jvol
 (3u} T [3] T [0]{s: th } d(vol)
^YOl
 {ou} T p [A] T [A] d(vol) r {u}
+ {<5u 7 }p J [A] 7 d(area) (C.23)
* area
Noting that the {00} is common in all of the above terms, and that its
terms are independent of each other, it may be cancelled out. Thus,
equation C.23 reduces' to":""'
DC e ]{u}  {F^} = [M e ]{u> + {?l r } (C.24)
where: [K ] = I [B] [D][B] d(vol) = element stiffness matrix
e Jvol
ir } * I [3] [0]{£^u> d(vol) = element thermal load vector
e J vol *
[M«] = p I [A] [A] d(vol) = element (consistent) mass matrix
' e J vol .
.2
{u} =fr{u}= acceleration vector (such as gravity effects)
a U
ny I T
{F* }  [A] {p> d(area) = element pressure vector
J area
112
Those elements which use a lumped sum mass matrix rather than a consistent
mass matrix are noted with the individual element description.
The element stresses are computed by combining equations C.3
and c.15 to jet:
M  CD]([B]{u}  { £th »
(C.25)
Mote that [S] is the straindisplacement matrix that must be specialized
for each stress calculation point (centroid, integration point, node point, etc,}
Virtual Work. Derivation for Thermal Analysis Elements
As before, the basic expression of virtual work is:
SU = sV
where: 511 = virtual internal work
5V s virtual external work
In thermal terms, the virtual work within one element is:
<5U
(C.26)
 I (5S> T
'vol
{Q v > d(vol)
(C.27)
where:
C
3T(x,y,z)
ax
(S>< J 3T(x,y, 2 )
3T(XvY,z)
>  vector of temperature
v
3Z
IP
s x
WJ=<
> = vector of heat flows
v. Q «J
113
7(x,y,z) = temperature at point x,y r z
Q = heat flew in the xdi recti en per unit area
Q = heat flew in the ydi recti on per unit area
Q_ = heat flew in the zdi recti an per unit area
The heat flows are related to the temperature gradients by:
wnere:
<Q.,i ■
[0]{S}
[D] 
KYY
,
KZZ
(C.2S)
The temperature distribution within an element is based on the assumed
temperature shapes:
T(x,y,z) = (M}'{T }
(C.29,
where: {N} = vector of shape functions
{!'} = nodal temperature vector
e
Then, {S} is related to {7 } using the definition of {S> and equation
C.29 to give:
{S} =
[3]{T e >
(c.3a)
wh
ere
[B] =
{— }
T
l 3y '
T
T
{ iN }
l 3X ;
Combim'na ecuations ■ C.27, C.28, and C20 and realizing that
114
the nodal temperature vector does not change over the volume of the
element,
? r [b] t i
Jvol
«U s {ST.}' [B]'CD][B] d(vol) {T } (C.31)
e Jvol e
Next, consider the virtual internal work associated with con
vection surfaces:
..]
5AT Q d(area) (C.32)
area
where n = :i the direction normal to the surface. AT is defined by:
AT = T(x,y,z)  T B (C.33)
where: T(x,y,z)  the temperature function evaluated at the
s
convection surface
T„ s temperature of the coolant (bulk temperature)
Note that T„ is a constant so that
SAT «T(x,y,z) (C.34)
s
The heat flow over the unit area is defined by:
Q n = h f AT (C35)
where h f = film, coefficient for heac. transfer of the surface. Combining
equations C.29, C.32, C.33, C.34, and c.35, and noting that {T g } does
not vary over the surfaced arid that Tg and h f are. assumed not to:
115
oU*{oT e } T h f 1 {N } T d(arga){T e >
area s
C5T e > T h f T 5 f {N > d(area) (c.36)
/ area
where {N } are the shape functions evaluated at the convection surface,
s
The internal heat generation rate effect is included by con
sider? na:
5V  J oT(x,y,z) q d(vol) (C.37)
where "of = the heat generation rate per unit volume. Combining equations
C.29 and C.37 and real vz4"ng that the nodal temperatures vector (T }
does not change over the volume of the element, and assuming that of
does not chance over the volume of the element,
5U={dT 8 > T q j {N} d(vol) (C.38)
J vol
The virtual internal work associated with a change of stored
energy is:
5U = I 5T(x,y,2)y d(vol) (C.39)
'vol
3 T f x v 7 )
where: y = pC — ' lV~ ! • total heat change per unit volume per
P 3 C
unit 'time
p = density
C = specific heat
t = time
116
Combining equations C.29 and C.39 and noting that {T } does not vary
over the element, and assuming that p and C do not vary over the
P
element,
oU = (6T e } T pC p J
vol
oU = (6T e } T pC p J (N}{N} T d(vol) {t a } (C.40)
where { y = ^ ty
The effect of the nodal heat flows may be considered by,
5V » (oT e } T {Q e ) (C.41)
where {Q } is the nodal heat flow vector.
Combining equations C.26, C.31, C.36, C.38, C.40, and C.41,
and noting that since {<5T } is an arbitrary set of virtual temperature
changes which may be cancelled out,
[K a ] + [K^] (y + [Cj{y = {Q^} + {Qp + {Q e } (C.42)
where: [K fi ] = J [B] T [D][B] d(vol)
70 = total element conduc
[K?] = h f f (NL HNL } T d(area) tivity matrix
e T y area
[C ] ■ PC J {N}{N} T d(vol) = specific heat (thermal
e " vol damping) matrix
{Q e } = h f T BjT {N I S } d ( area )
area
= total element heat
rn q, ••• r ,.,, ,/ ,x flow vector
CQ«} = q / {N} d(vol)
e Aol
This is the final temperature heat flow equilibrium equation. The
above definitions are used to develop the element matrices and vectors
117
■ STIF12  TWODIMENSIONAL INTERFACE ELEMENT
The displacement functions for the interface element can be sep
arated into the normal and tangential directions because they are basically
independent.
Tn the normal direction, when the normal force (F ) is negative,
the interface remains in contact and responds as a linear spring. As the
normal force becomes positive, contact is broken and no force is trans
mitted; unless KEYSUB(1)=1 , in which case asmall force is supplied to
prevent a portion of the structure from being isolated.
In the tangential direction, for F < arid the absolute value
of the tangential force (F ) less than or equal to (pF ), the interface
does not slide and responds as a linear spring in the tangential direction.
However, for F„ < and F > uF I , sliding occurs. Note that F„ is a
n s ' n 1 s
variable and if contact is broken, the tangential function degenerates
to a zero slope straight line through the origin Cor of slope K/10 , if
KEYSUBO)=l) indicating that no Cor little) tangential force is required
to produce sliding. These may be related to each other by yF  *
K(u  u  u , . . A where u .. . is the distance of sliding. Figure
s, s, slide) slide
C2 shows ■" the; forcedeflection relationships for this element.
Figure CI .
118
SLOPE* K/10°
If KEYSUB(l) = 1 j)
L
(«„}  («„)  4
:»
ulF.
SLOPE =■ K/10
If KEYSU3(1) = 1.
1
(O  (u )
s J s I
U r
For F < and for
n
initial loading
Figure C2. STIF12 ForceOeflection Relations
STTFI2 may have one of three conditions: in contact and not sliding,
in contact and sliding, or open. The following matrices are derived with the
assumption that 9 (theta) is input as 0.0.
1. In contact and not sliding  The resulting equilibrium
equation is:
L
K
K
K
K
K
K
stiffness matrix
K
K
U s,I
'n.I
r sl
nl
r *\
" Ku o
KA
<i r a s f + i r (c ' 43)
n
's,J
^ n,Jj
sJ
n
nJ
Ku.
KA
Displace Applied Element Load
ment Nodal Vector
Vector Force
Vector
119
where
K =
A =
F =
n
input stiffness
interference
normal force across gap
distance that nodes I and J have slid with respect to
each other
2» In contact and sliding  In this case, the element equilib
rium equation is:
K K
K K
Stiffness Matrix
r,
<
's,I
l n,I
's,J
si
>=<
vVi
nl
sJ
uF.
F n
I. nJ
KA
pF r
KA
Displace Applied Element
ment Vector Modal Load Vector
Force
Vector
where y = coefficient of friction.
(C.44)
3. Open  When there is no contact between nodes I and J, the
stiffness matrix and load vector are null matrices.
The stress pass of STIF12 always uses the latest possible informa
tion concerning gap status. Therefore, for noncnnverged iterations, it
may not agree with the reaction forces which are based on the previously
calculated stiffness matrix and load vector.
120
STTF32  20 CONDUCTING 3AR ELEMENT
The temperature function is a linaar polynomial of the form:
T(x) = C 1 + C 2 ;
(C.45)
wn
ere the element xaxis extends along the element axis
STTF42  20 ISOPARAMETRIC SOLID ELEMENT
The 'displacement shape functions are repeated here for convenience,
A local: coordtnatss&sSem fs developed as shown in Figure C3:
Y.v
(1,1)
(1,1)
(1,1)
(1,D
X,u
Figure C3. Local Coordinate System
121
It is seen that s and t vary between 1 . and +T. The basic, isoparametric
shapes yield the following set of shape functions:
U b (s,t) = 1(1  S)(l  tJUj + ^{1 + S)(l  t)Uj
+ \0 + s)0 + t)u ;< + Itf  s}(l + t)u L (C.46)
v b (s,t) = 1{1  s)(l  t)Vj + 1(1 + S)(l  t)Vj
. 1
1/,
^■0 + s)(i + t)v ;< i(i . sjq + t)v L
(C.47)
Mote that these shapes do not permit the edges to bend.
The extra (and optional) shapes are defined as
u e (s,t) = (1  s^Cj + (1  t 2 )c 2
v e (s,t) = (1  s 2 )c 3 + (1  t 2 )c 4
(C.48)
(C.49)
Their effect may be seen in Figure C4. c, through c, may be referred
to as node! ess variables. The total displacements are then:
u  u. + u
d e
v  v b + v e
(C.50)
(C.51)
Without extra shapes
With extra shapes
fi
gure C4. Effect of Extra Shapes
122
These displacement shapes are used to' generate a 12 by 12 stiffness
matrix. This matrix is then condensed to an 3 by 3 matrix, because there
are only 3 decrees of freedom to connect to the rest of the structure The
condensation is analogous to that associated with superelement generation.
The Toa <j vector "is also generated .with TZ. terms and. is then: condensed to a.
The mass matrix Ts consistent and is' generated as an 8.. bf.£
A 3 by 3 lattice of integration points is used with the numerical
(Gaussian) integration procedure.
Note that the extra shapes permit a parabolic deformation along an
element edge. Normally this is helpful in modeling a structure, but
occasionally it may cause a problem because of the incompatibility at the
adjoining edges of two different elements, i.e., a gap opens up or the
material "doubles up". The usage of the extra shapes is discussed in greater
detail in the User's Manual. The extra shapes are automatically deleted if
nodes K and L are the same (i.e. a triangle). This case then gives the same
results as a constant strain triangle.
The centroidal, integration point, and node point stresses' are com
puted by the procedure described at the beginning of this chapter (£quaticn c. 25 •]
Surface stresses may be requested for elastic isotropic materials.
Even though the development given below includes some orthotropic effects,
it is only valid for a few special cases of orthotropic materials. The
surface stresses for plane stress applications, are calculated by:
1. Computing the strain parallel to the fr^e surface:
u '
U T  u ,
I L x \C.zZ)
123
Where: u s displacement parallel to the free surface
L = distance between the two surface nodes
a * coefficient of thermal expansion (ALPX)
AT s difference between average surface temperature and the
reference temperature.
2. Setting the stress normal to the surface (a) to the applied
pressure.
3. Setting the stress in the z direction (a) to 0.
4. Solving for the remaining three quantities of interest
(e 2 , £, a, ) by use of the material property relationships. Specifically:
°1 " e l h + v xy °2 (C  53)
6 3 = " v xy (ff l + ff 2 )/E ;
(C.54)
e 2>('2 u xy e l )/E a {C  55)
where: E, = (E, + Ej/2.
a A j
E = Young's modulus in the* xdi recti on (EX)
E = Young's modulus in the ydirection (EY)
v  Poisson's ratio (NUXY)
*y
For the axi symmetric option, steps 1 and 2 above are the same.
Continuing,
3. Computing the hoop strain (£3):
T T T
U T + U J %
124
where: u, = radial displacement of node I
u, = radial displacement of node J
u g  radial displacement of the midpoint of side I J due to the
applicable extra shape function
R s radius of the midpoint of side I J
a^ s coefficient of thermal expansion in hoop direction (ALPZl
4. Solving for the remaining three quantities of interest (e^* a i »
a) by use of the material property relationships. Specifically,
a  £ 3 E z+ ( V+"xz v xy )q 2 + £ fxz E a (C.57)
3 1 '*
E.
it
a, s £, E. + a„v + a,v f— (C.58)
« =!i v !l v !i (C.59)
e 2 E a u xyE a VE 2
where: E s input quantity (E2)
v ■ input quantity (NUX2)
v = input quantity (NUYZ)
Plane strain analysis is the .same as axisymmetric analysis,,
except that step 3 is modified so that simply,
e 3 = a AT (C.60)
125
STIF45  30 ISOPARAMETRIC SOLID ELEMENT
The element formulation includes incompatible displacement
modes. A complete description of this technique is the threedimen
sional extension of STIF42. Either a 3x3x3 or a 2x2x2 lattice of
integration points is available for use with the numerical (Gaussian)
integration procedure. For nonlinear material properties (plasticity,
creep, or swelling), a 2x2x2 lattice is automatically used.
The principal stresses are calculated from the cubic equation:
x xy
T xy a y ' a
'xz
yz
T xz T yz a 2 ~ a
=
(C.61)
The three computed values of a are the three principal stresses
126
STIF52  30 INTERFACE ELEMENT
The Toaddeflection relationships for the interface element can be
separated into the normal and tangential directions since they are basically
independent. In the normal (element x) direction, when the normal force (F )
is negative, th& interface remains in contact and responds as a linear spring.
As the normal force becomes positive, contact is broken and no force is trans
mitted (unless KEYSU3(1 )=1 > then a small force is supplied to prevent a portion
of the structure from being isolated).
In the tangential directions, for F < and the absolute value of
n
the .tangential force (F ) less than or equal to (yF ), the interface does
not slide and responds as a linear spring in the tangential direction. How
ever, for F < and F > ^ilF I, sliding occurs. Mote that F is a variable
n s ' n ' n
and if contact is broken, the tangential function degenerates to a zero slope
straight line through the origin (or of slope k/10 , if KEYSUB(1 )=1 ) indi
cating that no (or little) tangential force is required to produce sliding.
Figure CS shows' the* force deflection functions" for this element
F nA
Sloce=k/10°
if KEYSUBOH
(u n )j(u n ) I+ GAP
F s*
yF ! 
Slope=k/10 Q
(if :<EYSUB(1) = 1
±5% tolerance
if KEYSU3(2)=1
< u s>j< u s>i
u F.
for F <
n
.5'''
Fiaure Co.
ForceDefl ection Rel ationships
127
STIF55  20 ISOPARAMETRIC HEAT CONDUCTING SOLID ELEGIT
The temperature functions used in STTF53 are a scalar form of
those developed for displacements in STIF42.
First, an element coordinate system is developed as shown in Figure Co.
Y
i
(1,1)
(1,1)
.(1,D
(1,1)
Figure C6~.
Element Coordinate System
It is seen' that s and t vary between 1. and +1. The basic isoparametric shapes
yield the following set of temperature functions:
T. Q (s,t) = l/4(ls)(lt)T r + l/4(l+s)(lt)Tj
+ l/4(l+s)0+t)T K + l/4(ls)(Ut)T L
The extra (and optional) shapes are defined as:
T e (s,t) = (ls 2 ) Cl + (lt 2 )c 2
(C.52)
(C.63)
128
C, through c may be r*farr*d to as nodal ass variables. The total
temperatures are then:
T = T. + T ( c  64 i
d e
These displacement shapes are used to generate a 5 by 5
stiffness matrix. A 3 by 3 lattice of integration points is used with
the numerical (Gaussian) integration procedure. This matrix is then
condensed down to a 4 by 4 matrix, because there are only four nodes to
connect to the r^st of the structure. The condensation is analogous to
that associated with superelement generation equation,' The load
vector is generated also with six terms and is then condensed down to
four. The damping ( specif icfheat) matrix is consistent and is also
reduced down from a 6 by..&.ta.aw4by 4.
129
APPENDIX D
COMPUTER DEFINITIONS AND COMMUNICATION LINKS
DEFINITIONS (UNIVAC 1100 COMPUTER)
The hardware organization of the 1110 (1100/40) and 1100/80
Systems differ from that of the 1106, 1108, 1100/10, and 1100/20
Systems. In some instances, different terms have been adopted for
functionally similar components. In such cases, to avoid confusion
and improve readability,, the 1108 term has, as a general rule, been
used throughout this document synonymously with the corresponding
1110 term, except where specific comments are made to the contrary.
11 08 type will be used to include the 1106, 1100/10, 1100/20, and
1108. 1110 type will be used to include the 1110 and the 1100/40.
The principal corresponding terms are:
1108
CPU
ACU
Control
Introductory
Registers (■
Definitions
bit
Binary digit.
value or 1 .
the functional
CICR)
mo
1100/80
CAU(plus IOAU)
CPU(plus
SPU
STU
CRS
GRS
IOU)
The fundamental unit of storage having the
Bits are grouped in bytes and words to form
manipulative units of storage devices.
byte A group pf adjacent bits usually operated upon as a unit;
can be 6, 9, 12, or 18 bits.
buffer On 1100/80 a high speed storage interface (4k to 16k).
storage
Executive The 1100 Series Executive System. A program that controls
or EXEC the execution of other routines. The Executive is the
principal interface between the user and the system as a
whole. It protects against undesired interaction of users
with each other or the operating system.
hardware Physical equipment, in the form of mechanical, magnetic,
electrical, or electronic devices, as opposed to software.
I/O Input/Output. The process of transferring information be
tween the central processor and peripheral, devices. I/O
devices include: magnetic tapes, magnetic disks, magnetic
drums, CRTs, card readers, printers, and punches.
mnemonic Word or term devised so as to aid the human memory. Includes
acronyms, such as TTY (telety pewriter) and error mnemonics,
such as PWRLOS (powerloss).
130
operating The 1100 Series Operating System. The entire set of system
system software available for the 1100 Series which is either a
part of or operates under the Executive system. This in
cludes the Executive system proper, compilers, utility
programs, subroutine libraries, and so forth.
software
system
user
word
A set of computer programs including the operating system
and user programs, as opposed to hardware.
The total 1100 Series hardware/software complex comprising
an integrated information processing installation.
An individual or organization that consumes services
provided by the system.
A sequence
capable of
(a word is
Systems).
of bits or characters treated as a unit and
being stored in a single main storage location
represented by 36 bits for the 1100 Series
Hardware Definitions
ACU
applica
tion
Availability Control Unit. A device used i n 11 08 type
Systems to isolate particular system components for main
tenance or system partitioning. The ACU, in certain
operating modes, can initiate autorecovery.
The total installation hardware configuration or a subset
resulting from partitioning that configuration via hard
ware or software.
auxiliary Supplemental storage, as opposed to main storage.' It is
storage not directly addressable by CPU(s) and is "accessible only
through an 1/0 interface. It includes magnetic tapes,
flying head magnetic drum, FASTRAND drum, disk, or
unitized channel storage.
break
point
CAU
central
group
central
site
channel
A feature whereby the CPU can be stopped or interrupted
when a particular main storage address is read, written,
or executed as an instruction.
Command/Arithmetic Unit. It is the 1110, 1100/40 equivalent
of the instruction processing portion of a CPU. A CAU does
not contain an input/output section, as does a CPU. There
fore, it must operate in conjunction with an I0AU in order
to access peripheral' subsystems.
The CPUs, CAUs, IOAUs, IOUs, ACUs, SPUs, STUs, and consoles.
The central group, main storage, and attached onsite
peripheral equipment in a particular application.
A data path for transfer of information between the central
group and 1/0 devices.
131
CPU The Central Processor Unit component on 1108 and 1100/80
Systems which executes all control and arithmetic functions.
The 1108 System CPU contains an input/output section for
access to peripheral devices.
CRT Cathoderay tube display. A televisionlike device that
presents data in visual form.
dual Two separate data paths for transfer of information between
channel the central group and a subsystem. The sub system control
unit must have dual channel capability.
IOAU The IOAU controls all transfers of data between the peripheral
devices and primary and extended storage. Transfers are
initiated by CAU under program control.
IOU The IOU controls all transfers of data between the peripheral
devices and primary and extended storage. Transfers are
initiated by CAU under program control .
interface The logical path between two connected nodes.
interlock A condition in which a peripheral unit is unable to perform
an executable command until the condition is removed by the
operator.
layered A hardware architecture wherein different parts of main
storage storage have different performance characteristics. On the
1110, and 1100/40, this refers to the fact that main storage
consists of primary and extended storage.
lineid Identification of the communications line to which one or
more remote terminals are attached. Line id is a unique
identifier of one to six alphanumeric characters assigned
by the installation.
main The generalpurpose high speed magnetic core, semiconductor
storage or plated wire (1110 only) storage of the system directly
addressable by the CPU, CAU, and IOAU/ IOU and serving
principally to contain executing programs.
mass Auxiliary storage which has random access capability, as
storage opposed to magnetic tape, for example. Includes any type
of flyinghead magnetic drum, FASTRAND drum units, disk,
and unitized channel' storage.
wordaddressable Mass storage which is capable of being
mass storage accessed in units of single words in
cluding any flyinghead magnetic drum,
and unitized channel storage. Word
addressable mass storage may be simu
lated on disk.
132
FASTRAND formatted Mass storage which is accessible in units
mass storage of 28 words Cone sector). This may be on
actual FASTRAND drum hardware, or may be
simulated on other mass storage devices.
The term FASTRAND in this manual refers
to the format, not the hardware device,
unless otherwise stated. This is the
most common mass storage format.
fixed mass storage Drum, unitized channel storage, FASTRAND
drum units, and disk units declared to
be fixed during the boot of the system.
This storage is considered to be perma
nent (online).
MP Multiprocessor. An application having two or more CPUs or
CAUs.
network All the nodes and interfaces in a system.
node A system component.
offline A condition in which hardware components are not under direct
control of the operating system.
online A condition in which hardware components are under direct
control of the operating system.
P  Program address register. A CPU control register which
register contains the absolute main storage address of the next
instruction to be executed. See Appendix A for numeric
conversions.
peripheral Hardware that is distinct from the CPU, IOAU/IOU and main
equipment storage, and which provides the system with increased
storage capacity, or with I/O capability.
remote Data terminal equipment that is time, space, or electrical!
site distant from a central site, and capable of information
exchange with the central site via communications lines.
siteid Identification of a remote terminal. Siteid is a unique
identifier of six alphanumeric characters assigned by the
installation to a terminal or group of terminals.
SPU System Partitioning Unit. A device used in the 1110 System
which permits offline maintenance of units, enables the
operator to logically partition the system into two or three
independent systems, and can initiate a recovery sequence
in the event of failure.
STU System Transition Unit. It contains the controls and
indicators for partitioning the SPERRY UNIVAC 1100/80
Systems into two independent systems. It also provides an
automatic recovery feature and system power control .
133
subsystem One or more peripheral units of the same type, plus a
control unit which is connected to an available I/O
channel. (.Can be a dual subsystem).
symbiont Relatively slowspeed devices, such as card readers, card
device "punches, and printers are controlled by symbionts and are
used to provide direct input to and output from the system.
system The hardward units of a system. They include CPUs, lOUs,
conponent CAUs, IOAUs, primary storage, extended storage, control
units, and devices and peripheral subsystems.
system
drjm/
dfsk
TTY
The mass storage unit to which the Executive is loaded.
The system drum/disk is usually unit zero of the specified
subsystem. The subsytem of the system drum/disk is
specified during system's generation. This specification
may be modified by the operator during tape bootstraps.
Teletypewriter equipment involving keyboard, printer,
and sending and receiving equipment. Used primarily as
a demand processing terminal.
unitized
channel
storage
Main storage which is treated as and accessed by
peripheral I/O hardware.
UP
Unit processor. An application having a single CPU,
or CAU/IOAU.
Software
Definitions
CPU/IOU,
backlog The collection of runs which has been entered into the system
and are held for facilities availability or unit directed
time start. Backlog resides on mass storage.
batch A mode in which runs are processed without any basic requi re
process ment for interactive manual data or controlled input during
ing processing.
break The division of symbiontdefined files into parts such that
point the output of completed parts may be initiated prior to run
completion. This procedure allows more efficient utilization
of printers and punches when large symbiont output files are
involved.
check Saves the run at a particular point in time for the purpose
point of subsequent restart in case of error or interruption.
deadline A batch run which is given certain schedule priorities to
run attempt run completion by a prescheduled time.
134
demand
process
ing
file
A mode in which run processing is basically dependent on
manual interaction (.typically from a remote terminal)
"timesharing".
during processing. Commonly known as
.An organized collection of data, treated as a unit, and
stored in such a manner as to faciliata the retrieval of
each individual data item. Files are retained on
auxiliary storage devices.
catalogued file A file known to and retained by the
Executive for a period of time not
necessarily related to the life of a
particular run, and retrievable by
runs other than the run which origi
nally created the file. In some cases,
a catalogued file may be accessed
simultaneously by two or more runs.
A transient file created by, accessible
to, and existing within the life of a
single run (as opoosed to catalogued
file).
logical The name associated with a system component. The logical
name name is not required to connote the system component with
which it is associated.
real time A mode of operation in which the system's response to input
process is sufficiently fast to influence the operation being con
ing trolled. In the real time mode the program generally has
exclusive use of a CPU/CAU. Generally, real time processing
is under the influence of independent inputs from one or
more communications devices. The real time mode may be
entered from either batch or demand mode.
temporary file
restart
run
run id
swapping
Resumption of processing a run from a checkpoint rather
than from the beginning of the run.
A group of tasks prescribed as a unit of work for the system.
A @RUN control statement must be the first card or image of
a run. A @FIN control statement is the last image.
Identifies a run to the Executive. Run id may consist of one
to six alphanumeric characters and is specified on the @RUN
control statement. If the specified run duplicates a run id
already in the system, the Executive modifies the newly sub
mitted run id to make it unique. When the run id is modified,
both the original and the modified runids are output to the
operator console.
The 1100 Series Operating System's method of moving low
priority runs from main storage to mass storage in order to
provide space to load higher priority runs into main storage
for execution.
135
symbiont A complex of Executive routines providing the user interface
with symbiont devices. Symbionts buffer the output so that
symbiont devices can handle the high speed output which the
cemtral processor provides. This allows system processing to
proceed at the higher internal and mass storage speeds rather
'than at the relatively slow speed of symbiont devices .
TSS Terminal Security System
System Definitions
bootstrap Act of loading (.booting) the Executive into main storage
along with certain other initialization functions which
vary depending on the type of bootstrap performed. Boot
strap is used synonymously with boot.
initial bootstrap The method wherein the operating sy stem
is read from the boot tape and copied onto
mass storage devices. At the conclusion
of the initialization, the Executive
control routines, called the resident
Executive, are read into main storage and
are given control .
recovery bootstrap The method wherein the Executive control
routines are read from tape, disk, or
drum and copied into main storage.
autorecovery A recovery bootstrap of the system taken
when a system malfunction or error is
detected. The recovery may be system
initialed (programmed recovery) or ACuV
SPU/STU initiated. Operator intervention
is not needed for either type.
panic The process of documenting portions of main and mass storage
dump for future analysis. Panic dumps are usually initiated by
the operator or the Executive following a system error.
system The process of tailoring the operating system to the parti 
genera cular hardware configuration and software requirements of a
tion site. The end result of a system generation is a tape that
contains a copy of the operating system in a form suitable
for loading into the computer systam (i.e., a boot tape).
zero stop A CPU/CAU stop initiated by the Executive due to either
software or hardware detected faults.
COMMUNICATION LINKS /
The transmission and reception of data to and from a computer
require a highly reliable electronic conversion process in most instances
In general, data are generated and processed by both terminals and com
puters in coded formats utilizing patterns of binary bits. Transmission
136
of data over communication Tines requires a conversion of data from an
electromechanical or magnetic storage format to electrical communication
signals . These signals represent tones that are audible only when used
to drive a suitable speakerlike or diaphragm device such as a telephone
receiver. On receipt, the signals or tones are reconverted to equiva
lent electrical energy to rerecord the data mechanically or magnetically.
The devices that perform this conversion process at both the
sending and receiving ends of a communication line are known as either
modems or Data Sets. (The word "modem" is an acronym for the function
"modulatedemodulate." Modulation is the conversion of impulses to
tones; demodulation is the reverse) . Data Sets are a specific type
of modem installed by Bell System companies. The modem, in effect, is
the telephone station through which a terminal talks to the timesharing
computer. In most cases, Data Sets include telephone instruments and
dials.
The actual connection of terminals to modems is accomplished in
either of two ways:
1. The terminal can be "hardwired" to the modem. This
indicates that the wiring of the terminal is connected
directly into the transmitter/ receiver unit.
2. The modem can incorporate an audio coupler . With this
approach, the connection is established between the
terminal location and the computer on an ordinary voice
grade dial telephone. The telephone handset is inserted
into the audio coupler of the modem, which then generates
or reads tones into or from the telephone instrument.
The hardwire installation is more reliable, of higher quality,
and of greater permanence. However, this approach requires profes
sional installation, represents a longerterm commitment, and is
less flexible.
By comparison, audio coupling is more subject to line interference
but far more flexible. With this technique, timesharing service can
be established or discontinued at any point where the user has a tele
phone instrument.
Timesharing transmissions can be carried over many different
kinds of communication lines. In general, line costs are directly
related to the transmission capacity and length of a given line .
The least expensive, lowestcapacity transmission line is known
as a halfduplex circuit. This is simply a circuit with two wires 
one signal line and a return, or ground  between two points. With
a halfduplex or twowire circuit, data can be transmitted in only
one direction at a time. Thus a terminal cannot be receiving data
from the computer while the operator is sending data. This type of
communication link has been used primarily for telegraphic service.
The next step up is to use a fourwire, or fullduplex, circuit .
This is the tyoe of connection normally established for telephone
137
conversions . Most timesharing services today use full duplex circuits.
These can be acquired either through dial service or on a leasedli.ne
basis. (With leasadlina service, a fullduplex ine is rented on a~
regular basis from telephone common carriers.) In general , a full
duplex line has the capacity to transmit or receive at a rate of up
to 2400 baud, or bits of data oer second. This is equivalent to
approximately 2^0 characters per second .
Consideration of this line capacity gives further dimension to
earlier discussions of terminal speed and automated transmission from
offline storage media. Recorded data can be transmitted at speeds
of up to 240 characters per second. However, even under automatic
operation, printing terminals are limited to 30 characters oer second
and a typist entering data directly from a keyboard is effectively
limited to seven or eiaht characters per second .
Where data transmission requirements are greater, additional lines
can be added. In general , communication lines with capacities greater
than full duplex are known as broadband service . Transmission capa
b ili ties are directly proportional to the lines available. Thus four
lines would make a transmission rata of 4800 baud available, eight
lines would carry 9600 baud, and so on. Services regularly available
from telephone carriers extend to 32 lines. However, users of time
sharing utility services will rarely require or encounter services
involving more than fullduplex lines.
In some cases, however, timesharing utilities do use a technique
known as multiplexing to concentrate transmission from a number of
users over the same telephone lines. Multiplexors are satellite
communication processors. (Minicomputers are often used for multi
plexing.) A large number of timesharing users, sometimes as many as
132, can be linked to a single multiplexing point. ..Their trans
missions are then carried from the multiplexor to the central computer
over either fullduplex or broadband lines. Typically, a multiplexor
will be set up in a city remote from the central computer . For
example, many timesharing companies operate computers in New York.
These organizations then establish multiplexing points in major cities
such as Chicago and Los Angeles, where users can link into the
national timesharing network through local telephone calls.
•U.S. GOVERNMENT PRINTING OFFICE : 19800328231/6531
138
N CO
0) s;
O j/i
ct
c
n
<t
(/
* — 1
1 CD
IT
X
CD
O
D
a
a
CD
c
N
c > (J
FEDERALLY COORDINATED PROGRAM (FCP) OF HIGHWAY
RESEARCH AND DEVELOPMENT
The Offices of Research and Development (R&D) of
the Federal Highway Administration (FHWA) are
responsible for a broad program of staff and contract
research and development and a Federalaid
program, conducted by or through the State highway
transportation agencies, that includes the Highway
Planning and Research (HP&R) program and the
National Cooperative Highway Research Program
(NCHRP) managed by the Transportation Research
Board. The FCP is a carefully selected group of proj
ects that uses research and development resources to
obtain timely solutions to urgent national highway
engineering problems.*
The diagonal double stripe on the cover of this report
represents a highway and is colorcoded to identify
the FCP category that the report falls under. A red
stripe is used for category 1, dark blue for category 2,
light blue for category 3, brown for category 4, gray
for category 5, green for categories 6 and 7, and an
orange stripe identifies category 0.
FCP Category Descriptions
1. Improved Highway Design and Operation
for Safety
Safety R&D addresses problems associated with
the responsibilities of the FHWA under the
Highway Safety Act and includes investigation of
appropriate design standards, roadside hardware,
signing, and physical and scientific data for the
formulation of improved safety regulations.
2. Reduction of Traffic Congestion, and
Improved Operational Efficiency
Traffic R&D is concerned with increasing the
operational efficiency of existing highways by
advancing technology, by improving designs for
existing as well as new facilities, and by balancing
the demandcapacity relationship through traffic
management techniques such as bus and carpool
preferential treatment, motorist information, and
rerouting of traffic.
3. Environmental Considerations in Highway
Design, Location, Construction, and Opera
tion
Environmental R&D is directed toward identify
ing and evaluating highway elements that affect
* The complete sevenvolume official statement of the FCP is available from
the National Technical Information Service, Springfield, Va. 22161. Single
copies of the introductory volume are available without charge from Program
Analysis (HRD3), Offices of Research and Development, Federal Highway
Administration, Washington, D.C. 20590.
the quality of the human environment. The goals
are reduction of adverse highway and traffic
impacts, and protection and enhancement of the
environment.
4. Improved Materials Utilization and
Durability
Materials R&D is concerned with expanding the
knowledge and technology of materials properties,
using available natural materials, improving struc
tural foundation materials, recycling highway
materials, converting industrial wastes into useful
highway products, developing extender or
substitute materials for those in short supply, and
developing more rapid and reliable testing
procedures. The goals are lower highway con
struction costs and extended maintenancefree
operation.
5. Improved Design to Reduce Costs, Extend
Life Expectancy, and Insure Structural
Safety
Structural R&D is concerned with furthering the
latest technological advances in structural and
hydraulic designs, fabrication processes, and
construction techniques to provide safe, efficient
highways at reasonable costs.
6. Improved Technology for Highway
Construction
This category is concerned with the research,
development, and implementation of highway
construction technology to increase productivity,
reduce energy consumption, conserve dwindling
resources, and reduce costs while improving the
quality and methods of construction.
7. Improved Technology for Highway
Maintenance
This category addresses problems in preserving
the Nation's highways and includes activities in
physical maintenance, traffic services, manage
ment, and equipment. The goal is to maximize
operational efficiency and safety to the traveling
public while conserving resources.
0. Other New Studies
This category, not included in the sevenvolume
official statement of the FCP, is concerned with
HP&R and NCHRP studies not specifically related
to FCP projects. These studies involve R&D
support of other FHWA program office research.
0005b7fl0